Chapter 3

CASD

CASD is an acronym for Computer Aided Scenario Design. The preprocessor CASD for the CFD simulator FLACS-CFD is used to prepare the input data, or job data, that defines a FLACS-CFD simulation. This comprises the: geometry model, computational grid, porosities, and scenario description.

This manual describes CASD 8, but the general functionality is in principle the same for earlier versions.

• 3.1    Overview

This section provides a general overview of the functionality in CASD, starting with an overview of how geometry is represented in FLACS-CFD.

• 3.1.1    Geometry in FLACS-CFD

Geometry is represented as a binary tree, with union and left difference operations between primitives and operations. The binary tree exists as an object that is part of a geometry file. When working with geometry in the Object window you will always see the geometry as a list of nodes (a node is an operation or primitive), this means that altough the underlying representation is a binary tree, you will never see it as such.

3.1.1.1 Geometry representation

Figure 3.1: Binary tree example

An example binary tree can be seen in the figure above. Operations are represented by circles, and primitives are represented by boxes. Primitives can have a separate representation known as the FLACS-CFD model, as illustrated by the stippled boxes in the figure. The standard model, i.e. not the FLACS-CFD model, is commonly referred to as the visualisation or CAD model.

The FLACS-CFD model can contain the following primitive types: boxes, cylinders, ellipsoids, CP8s and GTCs. These primitives will represent themselves in the FLACS-CFD model unless the FLACS-CFD model have been removed or replaced. An example of this can be seen in the figure above; the box will represent itself in the FLACS-CFD model. In the same example, the cylinder has an empty FLACS-CFD model and will therefore not exist in the FLACS-CFD model.

This allows you to have more advanced and visually pleasing geometry for presentation purposes, while insuring that the model used by the simulator only consists of simple geometric shapes that have been extensively validated. For mere visualisation purposes, it is also possible to have geometry in the visualisation model that has no FLACS-CFD representation, for example geometry to show an escape route.

The porosity calculator available in FLACS-CFD, FGC (Flacs Geometry Calculator), will default use the FLACS-CFD model if it is available, when calculating the porosities. When importing CAD models using geo2flacs the FLACS-CFD model is no longer generated, and the visualisation model will be used.

See also:

The section about the visualisation and FLACS-CFD model when importing geometry using geo2flacs. The section about the object window and primitive list.

• 3.1.1.2 Primitives

The following primitive types are supported by FLACS-CFD:

• •    Box

• •    Cylinder

• •    Ellipsoid

• •    General truncated cone (GTC)

• •    Convex polyhedrons (CP8)

• •    Torus

• •    Rectangular torus

• •    Mesh

They all share a number of basic properties as seen in Common primitive properties.

Table 3.1: Common primitive properties

• 3.1.1.2.1    Box In addition to the properties specified in Common primitive properties, the box primitive supports the properties specified in Box primitive properties.

Table 3.2: Box primitive properties

• 3.1.1.2.2    Cylinder In addition to the properties specified in Common primitive properties, the cylinder primitive supports the properties specified in Cylinder primitive properties.

Table 3.3: Cylinder primitive properties

• 3.1.1.2.3    Ellipsoid In addition to the properties specified in Common primitive properties, the ellipsoid primitive supports the properties specified in Ellipsoid primitive properties.

Table 3.4: Ellipsoid primitive properties

• 3.1.1.2.4    General truncated cone (GTC) In addition to the properties specified in Common primitive properties,the GTC primitive supports the properties specified in GTC primitive properties.

Table 3.5: GTC primitive properties

Figure 3.2: Definition of a general truncated cone.

• 3.1.1.2.5    Convex polyhedron (CP8) In addition to the properties specified in Common primitive properties, the CP8 primitive supports the properties specified in CP8 primitive properties.

Table 3.6: CP8 primitive properties

Figure 3.3: Definition of a convex polyhedron.

• 3.1.1.2.6    Torus A torus can be used to represent, for example, pipe bends. In addition to the properties specified in Common primitive properties, the torus primitive supports the properties specified in Torus primitive properties.

Table 3.7: Torus primitive properties

• 3.1.1.2.7    Rectangular torus (rtorus) A rtorus can for instance model a bent plate. In addition to the properties specified in Common primitive properties, the rtorus primitive supports the properties specified in RTorus primitive properties.

Table 3.8: RTorus primitive properties

• 3.1.1.2.8    Mesh Mesh is a generic primitive that can take any shape. In addition to the properties specified in Common primitive properties, the mesh primitive supports the properties specified in

Mesh primitive properties.

Table 3.9: Mesh primitive properties

• 3.1.1.3 Operations

There are two different operation types supported by FLACS-CFD:

• •    Union

• •    Left difference

They share a number of basic properties:

Table 3.10: Common operation properties

• 3.1.1.3.1    Union Named unions are also referred to as a group, and are visible to the user in the object window. Unnamed unions are hidden to the user, but are necessary to represent the geometry as a binary tree. Unions support the properties specified in Common operation properties.

• 3.1.1.3.2    Left difference A left difference operation is a boolean difference operation applied between two nodes. The nodes can be any combination of operations or primitives supported by FLACS-CFD. The operation is named left difference because the geometry is represented in a binary tree, as shown in paragraph Geometry representation, and it is the right node in the tree that is subtracted from the left node.

See also:

See paragraph Left difference under subsection Menu bar in this chapter for information about how to create left difference operations. Advice on creating left difference operations is included in the Geometry modelling section of the FLACS-CFD Best practice chapter.

• 3.1.1.4    Materials

Table 3.11: Material properties

3.1.1.4.1 UV types See UV types for a complete list of the different UV types supported in FLACS-CFD.

Table 3.12: UV types

• 3.1.1.4.2 Drape direction Only applicable in combination with the Drape UV type. Defines the direction in which the texture is draped.

• 3.1.1.5    Light

Lights can be defined in a FLACS-CFD geometry by naming a primitive ”Light”. Operations can not be used to define lights. Three different configuration parameters are supported by lights. The parameters must be added to the metadata property of the primitive. See Light configuration parameters for an explanation of the different parameters. Primitives can easily be converted to lights by using the functionality described in Convert. The lighting model supports only spherical lights and tube shaped lights, but any primitive can be converted to a light. For ellipsoids the spherical light model will be used, otherwise the tube shaped will be used, and fit to the primitives bounding box. Lights only have an effect when Realistic lighting is enabled.

Note:

Light calculations are both memory and computationally intensive, and adding too many lights to a geometry may cause a low frame rate and memory issues. Performance will depend heavily on the specification of your PC, and is affected by the available CPU power, memory size (RAM), and graphics card resources.

Table 3.13: Light configuration parameters

• 3.1.1.6    Realistic lighting

Enabling realistic lighting changes the lighting computations to be more physically based, modelling Fresnel reflection and conservation of energy. It allows modelling of many different types of surfaces based on the two material properties, roughness and metalness.

The roughness parameter models surface irregularities not captured by the normal map, and can be set from 0% to 100%.

Metalness does not have a range, a material is either metal or non-metal, also called dielectric. The main difference between metal and non-metal materials is that metal reflects more light, and has no diffuse light reflection. Metal also has colored reflection, such as gold or copper, as some wavelengths of light may be absorbed.

Realistic lighting is not used when drawing semi-transparent objects.

Figure 3.4: Ellipsoids with roughness of 0%, 25%, 50%, 75% and 100%. Front row is metal and back row is non-metal.

• 3.1.1.6.1    Sky light When both realistic rendering and the sky is enabled, the sky will be used as the main light source. The position of the sun and color of the sky will affect the appearance of geometry.

• 3.1.1.6.2    Reflections Enabling reflections increases the realism and gives more spatial awareness by making surfaces reflect other surfaces around it. This is based on a screen-space reflection technique, computed after the geometry shown on the screen has been rendered. This means that surfaces can only reflect what is currently shown on the screen, so where it would normally reflect things outside the screen, or reflect obscured objects, the reflection will be incorrect. Reflections are computationally demanding and can be turned off.

Figure 3.5: Example of reflection, making it clear the object is floating above the ground plane.

• 3.1.1.6.3    Bloom To emulate high dynamic range, colors above a certain brightness threshold, such as

lights or some specular highlights, will appear to glow. Bloom is always enabled when realistic light is enabled.

Figure 3.6: Example of bloom effect, where sun is reflected in a box.

• 3.1.2    System requirements

Please see the section on Hardware and software requirements regarding the graphics card requirements for running CASD.

In CASD, if insufficient OpenGL support is present, some aspects of 3D views may not work, for example the wireframe display. If updating the graphics driver does not help then a workaround to obtain wireframe views of 3D geometries is to start CASD with the Open Inventor-based viewer, see the following section.

• 3.1.3    Starting CASD

You start CASD by clicking the CASD icon in the RunManager window:

• Figure 3.7: The CASD desktop icon

or alternatively by executing the command:

• > run casd

on the command line in Linux. If CASD is unable to obtain a license when connecting to the FLACS-CFD license server, then an error message like “The application was unable to start correctly (0x0000142). Click OK to close the application.” will be shown. To resolve such a problem see the guidance about how to set up a network license or single user license.

• 3.1.4 CASD command line options

The following options can be given when starting CASD on the command line: Table 3.14: CASD command line options

Example:

Linux:

• >    run casd -noLock

Windows:

• >    casd -noLock

Alternatively, the options may be set permanently in the FLACS-CFD RunManager (click Options, then click Preferences). This will only apply if CASD is started from the RunManager.

• 3.1.5 The main window in CASD

Starting CASD 7 opens the main window.

Figure 3.8: The main window in CASD

The main window is divided into the following parts:

• •    The menu bar

• •    The tool bar

• •    The command input field

• •    The geometry window(s)

• •    The scenario menu

• •    The status field

• •    The status bar

These parts are described in the following subsections.

The geometry window and scenario menu are dockable and can be moved and resized within the CASD window by clicking in their top right corner or dragging them on the top border of their windows.

Attention:

When the dockable windows are in undocked state they may disappear when CASD looses focus (e.g. when activating a different program) and return only when CASD regains focus again. This behaviour is not a property of CASD but depends on the window manager and can be set in its options. In KDE, for example, launch kcmshell4 kwinoptions and then go to the Advanced tab and disable Hide utility windows. This setting can also be accessed via System Menu → Applications → Configure Desktop → Window Behavior → Window Behavior → Advanced → Hide utility windows.

• 3.1.5.1    The menu bar

The menu bar contains the following menus:

• •    File

• •    Geometry

• •    Grid

• •    Porosities

• •    View

• •    Options

• •    Macro

• •    Help

The options on the various menus are described in separate sections in this chapter.

• 3.1.5.2    The tool bar

The tool bar contains the following parts:

• •    Main section: provides shortcuts to several of the commands on the menu bar

– New, Open, Save, Save as, Import, and Result on the File menu

– Calculate and Verify porosities on the Porosities menu

• •    Graphics section: controls various features of the The geometry window

– View splitting

– Rectangle zoom

– Spinning (toggle on/off)

– Highlighting option, from filled only (0) to various degrees of contour highlighting (1-5)

• •    Utilities section: plan drawings and load filters

– Add plan drawings as a design guide

– Add load filters to load selected parts of a geometry

• •    Snap point section: Snap points are active points on objects and primitives

– Snap to corner

– Snap to edge

– Snap to face

• •    Layout buttons to activate different layouts, and a Save layout button to create a layout based on the current arrangement of the CASD main window components. See also the menu entry Options -Layout manager.

Note that the sections of the tool bar can be in different order, depending on the active layout. You can define several layouts, which not only set the content of the tool bar, but also the arrangement of the other components in the CASD main window.

• 3.1.5.3    The command input field

The command input field represents an alternative interface between the user and CASD, in addition to the regular menus on the menu bar. The control input field contains a scrollable command history list, and a current command context indicator (left side). To control the command history list from the keyboard use:

• •    UP: retrieves the previous line from the command history list

• •    DOWN: retrieves the next line from the command history list

• •    RETURN: processes the content of the command input field

Hence, you can choose whether to use a menu option on the menu bar, for example: File →Exit →Yes (to exit and save) or to execute, after typing or retrieving, the following command in the command input field: ∗ file exit yes yes

Command line input will in many situations be the most efficient way to work with CASD. Other sections in this chapter present additional examples on how to use this feature.

Up to ten of the most recently used commands are stored after the end of a session.

Examples: Using the command input field in CASD

• •    Select a box primitive in an object. The following command moves the box to (2, 2, 2), and causes the properties dialog to be shown

– ∗ edit properties 2 2

– This is because the position is not completely specified. You do not need to specify all parameters, but you must include all values for the parameter specified.

• •    If you want to edit one of the last parameters in the dialog, it is not necessary to specify all the parameters in front. The parameter name can be used to indicate which parameter to edit

– ∗ edit properties size 2 2 2 vol por 0.5

• •    You can also supply the answer to a question in the input field. To delete an assembly/instance, CASD will ask to confirm the operation. To avoid the question dialog, type the following command

– ∗ geometry delete yes

– or shorter: ∗ ge de y

• •    To direct the output from a list to a file, append the file name after the list command. For instance, to list geometries in the database, enter the following command, which will create the text file outfile.txt

– ∗ geometry list outfile.txt

• 3.1.5.4    The geometry window

The geometry window in the main window displays the geometry, the computational grid and scenario parameters. In addition to the options on the View menu, there are several ways of manipulating the view:

• •    Rotation: left-click

• •    Panning: CTRL+left-click

• •    Zoom: rotate mouse wheel

• •    Rectangle zoom: right-click and select Rectangular Zoom

• •    Splitting and closing views: right-click+SELECT

• 3.1.5.5    The status field

The status field in the main window contains information concerning the: active database, project, geometry, grid, and units.

• 3.1.5.6    Geometry window icons

Each geometry window has its own icon bar underneath.

Figure 3.9: Geometry window icons

The geometry window icon bar has following the following functions.

• •    Switch between walk viewer and fly viewer

• •    Selection mode on

• •    View mode on

• •    Store camera position

• •    Re-store camera position

• •    Seek to picked point

• •    View all

• •    Switch between parallel and perspective projection

• •    Turn axis on/off

• •    View along X axis

• •    View along Y axis

• •    View along Z axis

• 3.1.5.7    Cursor coordinate field

A cursor coordinate field is located to the lower left of the geometry window. In Select mode this field shows the position of the mouse cursor in the geometry. In View mode this field shows the position of the current snap point, which is set by performing a CTRL+left-click in the geometry window.

A right-click in the cursor coordinate field opens a context menu with options to copy the coordinate value to the clipboard, and to change the font in the field. Changes to the font, e.g. size or typeface, is saved in the user settings.

Figure 3.10: The cursor coordinate field and it's context menu.

• 3.1.5.8    Status bar

The status bar in the main window display information concerning

• •    The current model being visualised (FLACS-CFD or visualisation model)

• •    If any load filter is enabled

• •    The current unit in use

• 3.1.6 Files in CASD

CASD stores job data in a set of files. For the arbitrary job number 010100, the most important files are the:

• •    Header file, 010100.caj: ASCII file created by CASD; defines the cs, co, and cg files used by CASD.

• •    Geometry file, co010100.geo: binary file created by CASD; contains a list of primitives that define the geometry; used by FGC and Flowvis. The geometry file is also called the obstruction file, or co-file. It is not a direct input to the simulation, but it is used by FGC when generating the porosity file.

• •    Grid file, cg010100.dat3: binary file created by CASD; defines the computational mesh; used by CASD, Flacs, and Flowvis.

• •    Porosity file, cp010100.dat3: binary file created by the porosity calculator, FGC (typically from the Porosities menu in CASD); defines the porosities for each grid cell; used by Flacs and Flowvis.

• •    Scenario file, cs010100.dat3: ASCII file created by CASD; defines the general scenario (monitor points, output variables, fuel region, pressure relief panels, ignition position, etc.); used by CASD, Flacs, and Flowvis.

The File menu in the main window contains commands for creating, opening, and saving the various job files. See section Files in FLACS-CFD for further information.

• 3.1.7    Working with geometries in CASD

Implementing the geometry model in CASD is often the most time-consuming part of a project. For modern process facilities it may be possible to import the geometry from an existing CAD model, but for many installations the geometry must be constructed manually from drawings, photographs, etc.

A large project, such as a full probabilistic analysis, can involve hundreds of CFD simulations, and each simulation will typically produce 10 to 15 different files. Hence, it is important to organise the files in a well-structured manner.

The building blocks in a CASD geometry are instances of objects. The structure within an object is described in Geometry representation.

The list of information required to implement a typical process facility, such as an offshore oil platform or an onshore process plant, is quite extensive and includes:

• •    Plot plan

• •    Sectional drawings

• •    Piping plan

• •    HVAC layout

• •    Cable trays layout

• •    Framing plans

• •    Cladding

• •    Deck plan.

Most FLACS-CFD users find it convenient to define standardised axis directions, and the following convention is used by Gexcon for typical process facilities:

• •    East-West along the x-axis, with positive x towards the east.

• •    North-South along the y-axis, with positive y towards the north.

• •    Up-Down along the z-axis, with positive z pointing upwards.

This results in a conventional right handed coordinate system, where the lower south-western corner of the facility coincides with the origin (0,0,0).

Each object in a CASD geometry is assigned a material property, and each 'material' is assigned a colour hue from the 0 - 360° colour circle. Many FLACS-CFD users assign certain hues to various structural elements, and the following convention is used by Gexcon for typical process facilities.

Table 3.15: Colour convention used by Gexcon

A standardised colour scheme makes it more straightforward to review geometries from old projects.

• 3.1.8    Working with mesh type primitives

The traditional FLACS primitives like box and cylinder always represent a single solid object, but the mesh primitive can represent anything from a single surface or solid, multiple surfaces or objects, or part of an object or surface.

Mesh primitives are normally the result of importing CAD files when the shape could not be detected as any of the other primitive types.

For mesh primitives that represent solid objects, the orientation of normals on the surface of the mesh is used to determine what is the inside and outside of the mesh.

CASD will try to detect if the mesh is a closed solid, and this can be seen as the ”Is closed” property on the mesh primitive in the object window. If the mesh primitive is known to represent a solid object, but is not detected as such, the ”Force closed” option must be set. A mesh object that is not closed and not force closed, will not produce volume blockage!

In some cases, a single solid object will be represented as multiple mesh primitives. The menu option Merge mesh can then be used to merge the objects into one.

Conversely, a single mesh primitive can represent several objects. The menu option Split mesh or Convex decompose mesh can then be used to split the mesh into multiple mesh primitives.

Splitting a mesh may result in f.ex the inner surface of a hollow object being split into a separate mesh. This will then become a ”inside out” mesh and should be removed.

• 3.1.9    Representing geometry: on-grid and sub-grid scale obstacles

To appropriately model the effect of obstacles, it is important that the obstacles are geometrically well-represented on the chosen grid. In most practical situations, it will not be possible to represent smaller obstacles on the grid, however these should still be included in the geometry model since they may be treated by proper sub-grid models. Larger obstacles like the floor or ground, the ceiling, the walls and larger equipment will be resolved on-grid. Such objects may be repositioned so that their edges fall on grid lines, see Geometry considerations for the grid.

The most challenging geometries to represent properly are repeated obstacles of the same size and spacing as the chosen grid spacing. In such cases, consider changing the grid to achieve a better representation; if this type of geometry is dominant, then the accuracy of the result depends on the representation of these objects being good enough. In cases where such objects are not dominant, one may pay less attention to how the geometry is represented. For normal offshore modules there will be a range of sub-grid obstacles which are more or less randomly distributed in space.

A sub-grid obstacle is an object with a size of less than 2 control volumes (grid cells); for such an object, sub-grid contributions to turbulence and flame folding are applied. Bigger obstacles are called on-grid.

In many experimental setups one will find repeated obstacles of the same size. The basic research on gas explosions has focused on the effect of obstacle arrays, rather than on the effect of more realistic geometries. Both categories are important in order to be able to validate tools like FLACS-CFD.

• 3.2    File menu

  • 3.2.1    New

Shortcut: CTRL+N

Creates a new simulation job.

The New command in the File menu creates a new empty job. If there were unsaved changes to the current job, a dialog box is displayed, asking about saving the changes.

• 3.2.2    Open

Shortcut: CTRL+O

This command opens an existing set of simulation files. The default simulation files selection is defined in the header file (∗.caj).

The Open command in the File menu opens an existing job.

If the file name is entered in the command input field, the path must be encapsulated in apostrophes, for instance:

∗ open "../../Test/000000.caj"

If the command is selected from the menu, or if no name is specified in the command input field, the Open dialog box is displayed, where the path and file name can be specified.

By default, the file filter is set for selecting CASD header files (∗.caj). The file type filter can be changed to show geometry files (co∗.dat3, co∗.geo) or all files (∗.∗). CASD will then open all files with the same job number.

If there were unsaved changes to the current job, a dialog box is displayed, asking about saving the changes. CASD will display the contents of the geometry file in the graphic area after a file is successfully opened. The contents of the geometry file can be edited using the Edit File command in the Geometry menu.

When opening a simulation whose cs-file compatibility field is different than the most current version you will be asked if you want to update the file to the latest version. If you decline to update the file, it will retain its original value when saved.

• 3.2.3    Save

Shortcut: CTRL+S

Saves the current simulation job (that is, the various files that define the job).

The Save command in the File menu saves the current job.

• 3.2.4    Save as

Shortcut: CTRL+SHIFT+S

The Save As command saves the current job under a new (user-defined) name (job number).

• 3.2.5    Import

Imports some specifications from another simulation job (for example, grid file, scenario file, etc.).

• 3.2.6    Export

Exports the visible geometry in CASD to file with the provided format (for example ∗.obj files).

• 3.2.7    Exit

Shortcut: CTRL+Q

Exits the CASD program.

• 3.3    Geometry menu

CASD stores the geometry in geometry files (co-files). The commands in the Geometry menu in the main window, except the Edit File command, are available when connected to a database. The Save and Save as commands in the File menu writes the geometry to the geometry file.

• 3.3.1    Edit file

The Edit File command in the Geometry menu makes it possible to edit the geometry file (co file) for the open job.

• 3.3.2    Statistics

The Statistics menu item allows to compute various properties of the geometry, such as surface area and volume. The values can be determined for specific parts of the geometry, and the results can be grouped into user-defined categories. Overlapping parts of the geometry will be identified and not be counted twice.

Figure 3.11: The geometry statistics tool in CASD.

Note:

The Statistics menu item opens a graphical front-end to the cofile2 tool. For the time being, the older cofile (deprecated) tool is still included in the FLACS-CFD package and can be only used from the command line. Please note that regions are defined differently in cofile and cofile2.

• 3.3.2.1    Prefilter

The prefilter option allows to specify what geometry to include in the calculation, e.g. by primitive type or hue. The filter is specified in the same way as the Quick filter used in the Object Dialog. Any geometry not matching the filter will be disregarded and not influence the results. An empty filter will include all geometry.

• 3.3.2.2    Regions

Regions can be set up to include or exclude parts of the geometry based on their location. Each region is an axis-aligned bounding box around the geometry to be included or excluded. The union of the regions to be included reduced by the union of the regions to be excluded defines the total region for which the geometry statistics will be prepared. For example an L-shaped region can be defined either as two include regions, or one include region and one exclude region. The result will be the same.

Double-click a region to edit its size. The region will be displayed as a bounding box in the CASD geometry that can be interactively positioned and resized.

• 3.3.2.3    Categories

Several categories and subcategories can be defined. Each category has a name and a filter rule. The name is a user-defined text, and the rule is a filter like the Quick filter used in the Object Dialog. The result values for a subcategory will be the sum of the result for all primitives matching the filter rule in the category and any parent category.

To define a top-level category, make sure that no category is selected in the list and click Add category. To define a subcategory, select the parent category and click Add category. Double-click the category name or filter rule to edit it.

The following subcategories have been predefined for cylinders:

Table 3.16: Predefined subcategories for cylinders

• 3.3.2.4    Saving and loading setup

The prefilter, regions and category setup can be saved to a file or loaded from an existing one. Such a file can also be loaded by the cofile (deprecated) utility.

• 3.3.2.5    Counting

Depending on the size of the geometry, the size of the regions, and the complexity/number of overlaps in the geometry, the calculation can take some time. A progress bar is shown while the geometry is processed.

Note:

As a polygonal representation of the geometry may be used in the calculations, the resulting values may not be exact. In particular, cylinders that are

• •    overlapping other geometry, or

• •    are part of a left-difference operation, or

• •    are only partly within a counting region,

will be represented as an extruded hexadecagon when calculating the volume and area. The error is partly compensated, but deviations of a few per cent should be expected in such cases. Also, compensation is not feasible for all object combinations and operations.

When computing the length of primitives, the center line is used. Parts of the center line that intersect bigger primitives will not add to the length.

To view a report of the results, click the View report button. The results can also be saved to a text file.

• 3.3.3    Import CAD file(s)

CASD allows to run a geometry import procedure using geo2flacs entirely from the graphical user interface. The figure below shows the import dialogue.

Figure 3.12: Geometry import dialogue in CASD.

After adding the relevant files, the object type can be set in the drop-down menu for each file. Transformation parameters for rotation, translation and scaling can be filled in if necessary. These correspond to the geo2flacs options -r, -t, and -s, respectively. Also filtering, grouping, and alignment options can be specified. The alternative to running the geometry import from the GUI is to use the geo2flacs utility for manual geometry import.

• 3.3.3.1    Advanced options

The Advanced options button brings up a dialogue with some additional options that can improve the import in some cases:

Advanced options for DWG/DGN import

Table 3.17: Geometry import advanced options for DWG/DGN import.

Advanced options for RVM import

Table 3.18: Geometry import advanced options for RVM import.

Advanced options for geometry analysis

Table 3.19: Geometry import advanced options for geometry analysis.

• 3.4    Object window

The object window opens when choosing the menu item Edit File in the Geometry menu.

Figure 3.13: The object window in CASD.

The object window consists of 6 main GUI elements as seen in the image above. More information about each GUI element can be found below:

• •    Menu bar

• •    Tool bar

• •    Primitive list

• •    Properties widget

• •    Quickfilter

• 3.4.1    Menu bar

  • 3.4.1.1    File menu

The entries in the File menu of the object window are explained below.

• 3.4.1.1.1    Save The changes are stored internally in CASD and will be written to the file when you use Save or Save As from the File menu in the main window. Closing the object window without saving will drop all unsaved changes.

• 3.4.1.1.2    Exit Before closing the object window, CASD asks whether the object should be saved.

• 3.4.1.2    Edit menu

The entries of the Edit menu in the object window are explained below.

Remarks:

To use the shortcuts displayed in this menu, the input focus must be on the 3D view; click MOUSE+LEFT in the 3D view to activate it.

• 3.4.1.2.1    Undo ShortCut: CTRL+Z

The Undo command allows the user to undo a large number of the commands available in the object window.

The supported commands include, but are not limited to, the following

• •    Convert -> ∗

• •    Properties

• •    Translate

• •    Scale

• •    Add -> Box

• •    Add -> Cylinder

• 3.4.1.2.2    Redo Shortcut: CTRL+Y

The Redo command allows the user to redo a large number of the commands available in the object window. It supports the same commands as the Undo command.

• 3.4.1.2.3    Convert The subcommands under Convert allows the user to convert primitives to a box, cylinder, mesh, ellipsoid, terrain or light. If the primitive cannot be converted an error message will be displayed.

See also:

Light for the specification of a light.

• 3.4.1.2.4    Mesh tools The mesh tools menu is used when working with mesh type primitives.

• •    Split mesh - Split the mesh into multiple disconnected components.

• •    Merge mesh - Opposite of split mesh, combines the selected meshes into one mesh.

• •    Repair mesh - Fixes small holes, degenerate faces or singular vertices in the mesh.

• •    Convex decompose mesh - Split the mesh into convex parts.

• •    Make normals consistent - Reorient normals so they point out of the mesh in a consistent manner.

• 3.4.1.2.5    Auto-align geometry This will check alignment of the selected primitives against X- and Y-axes, and if not determined to be aligned, the entire geometry will be rotated around Z-axis so that the selected primitives become aligned. If already determined to be aligned, nothing will be done.

• 3.4.1.2.6    Properties (deprecated) Shortcut: P

The Properties command in the Edit menu changes the primitive properties if the selected node is a primitive. If you have selected a subtree containing only one type of primitives, the Properties command can be used for changing one or more parameters for all these primitives.

• 3.4.1.2.7    Translate Shortcut: T

Use the Translate command to move the selected subtree a specified distance per axis direction.

• 3.4.1.2.8    From To Shortcut: F

Use the From To command to translate a subtree so that one specified position, the base point, is moved to another position, the target point. A dialog box for specifying the two positions is displayed. A circle is displayed in the 3D view, indication the position being edited. CASD keeps a list of positions used in the object. By pressing CTRL++ or CTRL+-, you can parse this list. The coordinates in the dialog box are updated.

• 3.4.1.2.9    Rotate Shortcut: R

The Rotate command rotates the selected subtree. You must specify a base point for the rotation, the axis, and the rotation angle. As for the From To command, you can parse the position list using the CTRL++ or CTRL+- commands. If the rotation angle is not a multiple of 90 degrees then CASD will warn about creating objects that are not grid-aligned.

• 3.4.1.2.10    Scale The Scale command scales the selected subtree. The origin for the scaling, and the scaling factor must be set. The position list can be parsed using the CTRL++ or CTRL+- commands before selecting Scale. The origin can be set by clicking CTRL+MOUSE+LEFT.

• 3.4.1.2.11    Scale XYZ Shortcut: SHIFT+S

The Scale XYZ command scales the selected subtree independently in each axis direction. The origin for the scaling, and the scaling factor must be set. The position list can be parsed using the CTRL++ or CTRL+-commands before selecting Scale XYZ.

• 3.4.1.2.12    Delete subtree Shortcut: Delete

The delete subtree command deletes all selected nodes in the primitive list and their children.

• 3.4.1.2.13    Delete node Shortcut: Backspace

The delete node command deletes all selected nodes in the primitive list but will not delete any children unless they are explicitly selected.

• 3.4.1.2.14    Mark Shortcut: CTRL+M

The Mark command is used when creating Left difference objects. It is possible to mark one or more nodes. Marked nodes are used as the positive part when adding a left difference operation. In order to mark nodes the user must select one or more nodes and trigger the Mark command.

See also:

The Advanced left difference operations section for example usage of the Mark command.

• 3.4.1.2.15    Duplicate Shortcut: D

The Duplicate command in the Edit menu duplicates the selected primitives and operations. You are asked to enter the number of copies, and the distance between each copy in the three axis directions.

See also:

The Duplicate command in the Geometry menu duplicates the selected instance.

Creating pipe bundles

Start with creating one cylinder with the appropriate diameter, length and direction. Use the Duplicate command in the Edit menu to duplicate the cylinder in one direction. Use the same command once more to duplicate the resulting row of cylinders in the other direction.

If you need to change some parameters for all the cylinders, select all the primitives and use the Properties command. If you want to change the distances between the cylinders, this can be done by scaling all the primitives. Afterwards you can use the Properties command to reset the cylinder diameters and lengths.

• 3.4.1.2.16    Material Shortcut: M

The Material command in the Edit menu edits the material name for the object. You must enter an existing material name. This action is only enabled when connected to a geometry database.

• 3.4.1.2.17    Open material editor Shortcut: Shift+N

Opens the ”Edit materials” dialog that shows all materials available to the object or geometry.

• 3.4.1.2.18    Open selected material Shortcut: Ctrl+Shift+C

Opens the material specified for the selected primitive for editing.

• 3.4.1.2.19    Change color This command allows the user to change the color of primitives and operations. The dialog that is opened by this command also allows the user to set the transparancy (Alpha channel). The color can be input as HSV, RGB or through the color picker.

• 3.4.1.2.20    Copy Shortcut: CTRL+C

This function copies the selected primitives and operations to the system clipboard.

• 3.4.1.2.21    Cut Shortcut: CTRL+X

This function cuts the selected primitives and operations and places them on the system clipboard.

• 3.4.1.2.22    Paste Shortcut: CTRL+V

This function pastes primitives and operations that was previously stored in the clipboard by copy or cut.

• 3.4.1.2.23    Remove FLACS-CFD geometry This will remove the FLACS-CFD representation, and have the same effect as deleting primitives from the FLACS-CFD model.

• 3.4.1.2.24    Reset FLACS-CFD geometry This will reset the FLACS-CFD representation back to the default representation of the selected primitives. If for example the FLACS-CFD representation has been removed, this can be used to bring it back. For Mesh primitives, you can choose to use Mesh Curvature Analysis when creating the FLACS-CFD primitives.

• 3.4.1.2.25    Replace geometry with FLACS-CFD geometry This will replace the selected visualisation primitives, with their corresponding FLACS-CFD representation, or remove them if the FLACS-CFD representation is empty.

• 3.4.1.2.26    Edit FLACS-CFD geometry The action (shortcut F4) can be used to switch between editing the visualisation model and the FLACS-CFD model. This will show the two models side by side, and the view currently being edited will be highlighted.

When the view is changed the selection in the current view will be used to set the initial selection in the new view.

In most cases it should be sufficient to edit the visualisation model. Any additions or removals to the visualisation model will also affect the FLACS-CFD model. Removing nodes from the FLACS-CFD model will only affect the FLACS-CFD model and not the visualisation model.

To add Primitives in the FLACS-CFD model the user must be editing the FLACS-CFD model, and a single node must be selected in the primitive list. Anything added will then become part of the FLACS-CFD representation of the currently selected visualisation primitive.

• 3.4.1.2.27    Group Creates a group (named union) containing the selected primitives and operations. This will prompt the user for a group name, and put the selected items under a new top-level group.

• 3.4.1.2.28    Ungroup Removes the selected group or the parent group of the selected primitives. The primitives in the group will not be removed.

• 3.4.1.2.29    Create instance... Selected primitives will be converted to an instance object, which then can be duplicated with minimal overhead. This is useful if the geometry include a large number of identical objects, e.g., trees in a forest, as it will speed up drawing, reduce memory consumption and reduce the size of the geometry file.

• 3.4.1.2.30    Replace instance with geometry The selected instance will be converted to a normal primitive, i.e. made unique.

• 3.4.1.2.31    Edit instance Opens a new object editor window where a selected instance object can be edited. This will update all the duplicates of the instance object in the geometry model.

• 3.4.1.2.32    Export to terrain

Allows the user to export all nodes to a terrain .tri file. See Terrain import in CASD for more information about terrains.

• 3.4.1.3    Add menu

The Add menu allows to add primitives to the object. The different primitives and operations are described below.

Remarks:

To use the shortcuts displayed in this menu the input focus must be on the 3D view; click MOUSE+LEFT in the 3D view to activate it.

• 3.4.1.3.1    Box Shortcut: B

The Box command in the Add menu adds a box to the end of the primitive list. A dialog box for defining the box parameters is displayed. See Box for a definition of the parameters.

• 3.4.1.3.2    Cylinder Shortcut: C

The Cylinder command in the Add menu adds a cylinder to the end of the primitive list. A dialog box for defining the cylinder parameters is displayed. See Cylinder for a definition of the parameters.

• 3.4.1.3.3    Ellipsoid Shortcut: E

The Ellipsoid command adds an ellipsoid to the end of the primitive list. A dialog box for defining the ellipsoid parameters is displayed. See Ellipsoid for a definition of the parameters.

• 3.4.1.3.4    CP8 The CP8 command adds a convex polyhedron to the end of the primitive list. A dialog box for defining the convex polyhedron parameters is displayed. See Convex polyhedron (CP8) for a definition of the parameters.

• 3.4.1.3.5    GTC The GTC command adds a general truncated cone to the end of the primitive list. A dialog box for defining the general truncated cone parameters is displayed. See General truncated cone (GTC) for a specification of the primitive type.

• 3.4.1.3.6    Torus The Torus command adds a torus to the primitive list. See Torus for a specification of the primitive type.

• 3.4.1.3.7    Rectangular torus The Rectangular Torus commands adds a rectangular torus to the primitive list. See Rectangular torus (rtorus) for a specification of the primitive type.

• 3.4.1.3.8    Left difference Shortcut: L

The Left Difference command adds a difference operation at the end of the primitive list. The marked nodes (Mark) are treated as the solid part of the operation, while the selected nodes are treated as the minus part. Both the solid and minus part of the left difference operation can be a collection of primitives and/or operations. When more than one node is marked as the solid part of the operation a named union will be created. A named union will also be created if more than one node is selected as the minus part of the operation.

Note:

One full grid cell is required inside the solid walls around “left difference holes” to ensure that the walls do not leak. In case of “minus cylinders” inside a solid cylinder, at least two CVs are needed, whereas one CV is sufficient for minus cylinders inside a box.

See also:

Advice on creating left difference operations is included in the Geometry modelling section of the FLACS-CFD Best practice chapter. A specification of the left difference operation can be seen in the Left difference paragraph.

• 3.4.1.3.9    Copy Shortcut: SHIFT+C

The Copy command adds a copy of the selected primitives and operations.

• 3.4.1.3.10    Object Shortcut: O

The Object command adds a copy of a specified object.

• 3.4.1.3.11    From file Adds primitives and operations from a geometry file.

• 3.4.1.4    Select menu

There are several ways to select multiple primitives in an object window, and these are accessible in the Select menu. The entries of the Select menu are explained below. Later, it will also be explained how to select primitives with the mouse.

• 3.4.1.4.1    Bounding box Shortcut: CTRL+B

This command lets you define a bounding box, and all primitives within it will be selected. If subsequently using the Cut or Copy operation, primitives intersecting the bounding box will be cut or copied at the intersection plane. For example the Cut operation can be used to cut a portion out of a Box primitive when it is partly overlapped by a bounding box.

• 3.4.1.4.2    Filter This command will set up a filter in the same way as the load filter in the main geometry view. Any primitives matching the filter rules will be selected.

• 3.4.1.4.3    All Shortcut: Ctrl+A

Select all primitives.

• 3.4.1.4.4    Invert Shortcut: CTRL+I

Selects all primitives not currently selected.

• 3.4.1.4.5    Stack Shortcut: CTRL+TAB

This command will parse (cycle through) the list of selected primitives or subtrees if more than one is selected.

• 3.4.1.4.6    Group Shortcut: CTRL+|

Will select the first named group of the selected primitive or operation.

• 3.4.1.5    View menu

The entries of the View menu in the object window are explained below.

• 3.4.1.5.1    The XY, XZ and YZ views Shortcut: Z

Shortcut: SHIFT+Z

Shortcut: Y

Shortcut: SHIFT+Y

Shortcut: X

Shortcut: SHIFT+X

The option XY View and XZ View display a projection of the geometry in the XY and XZ planes respectively. The options YZ East View and YZ West View display a projection of the geometry in the YZ plane along the positive and negative Y-axis respectively.

• 3.4.1.5.2    3D View Shortcut: 3

The 3D View option displays a default 3D view of the geometry.

• 3.4.1.5.3    Maximize Shortcut: SHIFT+M

The option Maximise maximises the visible window to display the entire geometry.

• 3.4.1.5.4    Axis Shortcut: A

The Axis option turns axis display on and off.

• 3.4.1.5.5    Terrain Toggle on/off terrain visualisation.

• 3.4.1.5.6    Grid Display This function has no effect in the object window.

• 3.4.1.5.7    Annotation This function has no effect in the object window.

• 3.4.1.5.8    Draw Style Different options are available in this menu:

• •    Off: The geometry will not be displayed.

• •    Default: Geometry is drawn according to database/primitive settings.

• •    Opaque: All geometry will is drawn opaque.

• •    Semi-transparent: All geometry is drawn semi-transparent.

• •    Wireframe: Only the edges of the objects will be drawn.

• •    Wireframe and default: Combination of above descriptions.

• •    Wireframe and opaque: Combination of above descriptions.

• •    Wireframe and semi-transparent: Combination of above descriptions.

• •    Realistic: Enable realistic lighting.

• •    Use textures: Enable use of textures and normal/roughness/metalness maps on geometry.

• •    Use reflections: Enable reflections (only available when realistic lighting is enabled).

• •    Use shadows: Enable shadows (only available when realistic lighting is enabled).

• •    Show sky: Show skydome and use sky light instead of head light if realistic lighting is enabled.

• 3.4.1.5.9    Fixed vertical axis When turned on it is not possible to rotate across +Z.

• 3.4.1.5.10    Fixed near plane In some situations parts of the geometry may disappear when they are very close to the camera. Toggling this function will fix this problem.

• 3.4.1.5.11    Hide/Unhide The actions in this menu makes it possible to hide one or more primitives from the 3D view. When hiding a primitive it will become grayed out in the Primitive list.

See also:

Please note there is also a global option to toggle on/off the show/hide functionality. See Toggle Hide Objects for more information.

• 3.4.1.5.12    Flacs view Enables and disables the Flacs view window.

• 3.4.1.6    Macro menu

The entries of the Macro menu in the object window are explained below. For more information about CASD macros see section Macro menu (deprecated).

• 3.4.1.6.1    Run Read a macro file defining a single object.

Attention:

Macro files generated by Write Object have to be read using the Run command from the Macro menu in the CASD main window.

• 3.4.1.6.2    Record Writes all commands given to a user-specified macro file.

• 3.4.1.6.3    Write Object Writes a macro file containing the current object.

Attention:

Macro files generated by Write Object have to be read using the Run command from the Macro menu in the CASD main window.

• 3.4.2    Tool bar

The available actions are in large parts identical to those described in section

CASD - The main window in CASD - The tool bar. The actions that are only available in the object window is described below.

• 3.4.2.1    Toggle Hide Objects

Shortcut: F8

When triggered this will enable/disable show and hide functionality for this object window.

• 3.4.3    Primitive list

The primitive list shows all primitives in an object. It will show the primitive name and the type for each primitive. Groups are shown with bold text. Primitives that are shown in italic text are the FLACS-CFD model; see Geometry in FLACS-CFD for more information about the difference. Primitives that have an asterisk behind the name has an empty FLACS-CFD model.

• 3.4.4    Properties widget

Allows you to quickly edit properties for the selected primitives and operations. When multiple primitives and operations are selected only intersecting properties will be shown. This feature replaces the deprecated Properties dialog.

For an overview of the different properties that can be set please see section Geometry in FLACS-CFD of this chapter.

• 3.4.5    Quickfilter

This command will set up a filter for selection, but defined by a string instead of the user interface as in the filter command. The available filters are:

Table 3.20: Quick filter syntax

The filter types can be combined using and and or operators and inverted using the not operator. For example:

box and (hue = 120 or length > 2)

selects boxes that are green or have length greater than two,

cylinder and not aligned

selects cylinders that are not axis-aligned.

A GTC is considered (axis-) aligned if its direction vector points along one of the coordinate axes. A CP8 is axis-aligned if three of the vectors are axis-aligned (those that span the origin corner if the CP8 were a box).

The direction of a cylinder is given by its axis, a GTC's direction is given by the direction vector, and for a box or ellipsoid the length dimension (the one with greatest extent) determines the direction; if the two maximum extents of a box or ellipsoid are equal then no direction will be defined. Also for a CP8 the direction is undefined and will not match direction x/y/z.

• 3.4.6    3D view

  • 3.4.6.1    Selecting primitives with the mouse

Besides the methods for selecting primitives that were explained above, it is also possible to use the mouse. To select primitives, Selection mode has to be enabled; it has the same icon as is used in the

geometry window. Left-clicking on a primitive will select it. By holding down CTRL and left-clicking several primitives successively, you can select multiple primitives. If you want to select a group of primitives that can be framed by a rectangle, you can press SHIFT on the keyboard and hold down the left mouse button while drawing a frame around the group of primitives that you want to select. See the image below for an example. When using this technique for selecting groups of primitives, it is important that there are no other primitives in front or behind of the intended group within the frame, otherwise these will be selected as well.

Figure 3.14: Multi-selection of primitives. Left: create a selection window with the mouse while holding the SHIFT key; right: all primitives in the selection window are selected.

Note:

The same ways of selecting primitives with the mouse also work in the geometry window.

• 3.5 Grid menu

The simulation volume is divided into grid cells (control volumes) by three sets of grid planes, one in each axis direction.

There is always a current grid working direction, and a selected region of grid planes in this direction. The current working direction is shown in the message area. The lines indicating the selected region are highlighted in the viewer.

• 3.5.1    Quick grid

Shortcut: CTRL+G

Using the Quick grid setup, it is possible to quickly create a grid with a core region covered by cells of a uniform size, surrounded by a stretched region where grid cells may vary in size.

Figure 3.15: The Quick grid setup window

The Quick grid setup window is divided in 4 sections:

• •    the boundaries and cell sizes for the core region are defined in metres in the first two sections,

• •    the stretched region of the grid is defined in metres in the third section, and

• •    information about the generated grid is shown in the fourth section.

Most parameters in the Quick grid dialogue require three values, associated with the X, Y and Z axes in that order. Values can be entered using the keyboard, the mouse scroll wheel, or by clicking the arrow buttons on the input field.

The values for the three axes are independent unless stated otherwise. If a relationship between two or more parameters is defined and no axis is specified, then the described relationship applies to each axis. For example, the expression (Cell size) * (Number of cells) = (Actual maximum) should be interpreted as

Note that it is possible to enter combinations of values into the Quick grid dialogue which cannot be used to define a grid that satifies the Quick grid requirements. When this happens, an error message is displayed, and the field that should be adjusted is highlighted in red. Adjusting the stretched domain usually solves this. When a scenario is saved and a grid is generated using the quick grid setup, the configuration parameters for the quick grid are saved in a ”quickGrid{jobnumber}.json” file. When the scenario is reopened in CASD, this settings file is used to populate the quick grid setup. If a scenario with no associated quick grid settings file is opened in CASD, then CASD will try to set appropriate quick grid settings. These settings may not be appropriate and should be checked.

See also:

Recommended grid configuration provides recommendations for defining grids appropriate for specific scenarios.

Below follows a short description of the various parameters.

• 3.5.1.1    Core domain

Minimum The location where the core domain starts in this dimension.

Maximum The highest coordinate for the core domain in this dimension.

Actual maximum The location where the core grid actually ends; it is given by the smallest multiple of Cell size that is larger than or equal to Core domain - Maximum.

Uniform grid If checked, the value of Cell size for the Y and Z axes is set equal to the value for the X axis. Same for the Max factor and Max cell size parameters.

Cell size If selected, the cells in the core domain are guaranteed to have exactly the specified size. The value of Number of cells is computed automatically.

Number of cells If selected, the core domain is guaranteed to have exactly the specified number of cells. The value of Cell size is computed automatically. If Uniform grid is checked, the Cell size for the X axis is computed automatically, and the value is used to determine the Number of cells for the Y and Z axes.

• 3.5.1.2    Stretched domain

Stretch domain If checked, the core domain is surrounded by a stretched domain. The size and the number of cells in the stretched domain are computed automatically. The size of the cells in the stretched domain is guaranteed to be larger than or equal to Cell size.

Minimum The location where the stretched grid starts. Must be less than or equal to Core domain -Minimum. If equal to Core domain - Minimum, no stretched domain is generated on the low side of the core domain.

Maximum The location where the stretched grid ends. Must be greater than or equal to Core Domain -Maximum. If less than or equal to Core domain - Actual maximum, no stretched domain is generated on the high side of the core domain.

Max factor The ratio between the size of two neighbouring cells is guaranteed to be less than or equal to this value. If Uniform grid is checked, the Max factor is the same for all the three axes. Otherwise, a specific Max factor can be defined for each axis. Only values between 1.0 and 2.0 are allowed. Suggested setting: 1.2.

Max cell size If enabled, the size of a cell is guaranteed to be less than or equal to the specified value. If Uniform grid is checked, the Max cell size is the same for all three axes. Otherwise, a specific Max cell size can be defined for each axis. This value must be larger than or equal to Core domain - Cell size.

See also:

Grid domains for more information about core domains and streched domains.

• 3.5.1.3    Grid information

Memory consumption An estimate of the amount of memory required by FLACS-CFD to calculate a simulation on the resulting grid.

Core aspect ratio The ratio between the largest and the smallest dimension of cells in the core domain. If Uniform grid is checked, the core aspect ratio should be exactly 1.0. The core aspect ratio should never exceed 100, and a value of 1.0 is recommended for explosions, see the recommendations for configuring the grid.

Min cell The size of the smallest cell in the grid.

Max cell The size of the largest cell in the grid. If Max cell size is enabled, this value is guaranteed to be smaller than or equal to Max cell size.

Actual max factor The actual maximum ratio between the size of two neighbouring cells. This value is guaranteed to be smaller than or equal to Max factor.

• 3.5.2    Check Grid

Shortcut: CTRL+SHIFT+G

The Check Grid menu choice opens a tool that can help to evaluate the quality of the current grid by checking it against recommendations in the grid guidelines. Please be aware that scenarios that include many scenario items might result in conflicting guidelines, which means that not all the recommendations can be fulfilled.

Note:

The evaluation does not consider the scenario geometry which might require additional recommendations according to the guidelines.

In addition to information about scenario type and items (leaks, panels, monitor points, fuel regions, etc.) read by the tool from the scenario setup, it is possible for the user to define a region of interest and confinement (i.e., if the scenario is confined by geometry on any sides). In addition, the user can set the ground level to exclude recommendations in negative Z direction that are not relevant as the grid is normally not extended below the ground level.

Based on the input from the scenario and the user, the tool will define a set of recommendations based on the grid guidelines, and test these recommendations against the current grid. The results are listed in a table as shown in the image below.

Figure 3.16: Example of the grid check dialog with recommendations for a simple fire scenario with a single jet leak. The white box in the 3D View represent the domain area related to the recommendation highlighted in blue.

Note:

The scenario needs to include a fuel region, a jet leak or a pool for the grid checker to be able to compute a core domain needed for generating a set of recommendations.

The columns in the table contains information related to each recommendation:

Status: Indicates if a recommendation is broken or OK.

Source: Indicates what triggered the inclusion of the recommendation (e.g. a specific scenario item, or if this is a general recommendation).

Guideline: Specifies the recommendation, e.g., that the number of cells in a defined area should be higher that a given threshold value.

Threshold: Specifies the threshold for the recommendation.

Domain: Specifies the target area for the recommendation, e.g. a range for a spesific grid axis, an area or a volume. When clicking on a row, the target area is visualized in the 3D view as a white line, rectangle or box, depending on the shape of the target area.

Result: If the recommendation failed, this column will show the current value so that it can be compared to the threshold value.

Note:

The check grid tool is provided to help the user setting up a grid that follows the grid guidelines, but although a grid does not fail any recommendations in the grid check dialog this does not guarantee that the grid follows all the grid guidelines. It is the users responsibility to make sure that a grid is following the guidelines for a given scenario.

• 3.5.3    Simulation volume

The Simulation volume command allows adjustment of the extent of the simulation volume in the three coordinate directions. If the volume is increased, the original grid planes are kept and one additional plane is added in each direction. If the volume is decreased, planes outside the new volume are deleted and new planes are created at the volume borders.

• 3.5.4    Direction

The Direction command changes the working direction. Legal inputs are x, y or z. The Grid menu commands Region, Add, Position, Move, Delete, Smooth, Stretch and List are implemented for grid planes in the working direction.

• 3.5.5    Region

The Region command substitutes the selected grid planes with a new set of grid planes and requires the new number of control volumes in the region to be entered.

• 3.5.6    Add

The Add command adds a new grid plane in the working direction and requires the coordinate value for the new plane to be entered.

• 3.5.7    Position

The Position command allows the position for the selected grid plane to be edited.

• 3.5.8    Move

The Move command moves the selected grid plane(s) a specified distance.

• 3.5.9    Delete

The Delete command deletes the selected grid plane(s).

• 3.5.10    Smooth

The Smooth command substitutes the selected grid planes with a new set of grid planes.

When the Smooth command is implemented, the sizes of the control volumes at each end of the region remain unchanged and sizes of control volumes between them is varied gradually, see the example in Grid guidelines. This function is typically used when refining the grid around a leak.

• 3.5.11    Stretch

The Stretch commands substitutes the selected grid planes with a new set of grid planes. This is particularly useful when stretching the grid towards the domain boundaries.

The Stretch command has two sub-choices:

• •    Negative Direction (typically used at the boundaries at the negative end of the axis)

• •    Positive Direction (typically used at the boundaries at the positive end of the axis)

The size of the control volume at one end of the region is required (the default is the current size). The factor by which the sizes of the control volumes in the specified direction should be increased or decreased is also required.

Attention:

Stretching of the grid should be avoided in areas of the simulation domain where the main combustion takes place. The flame model in FLACS-CFD in areas where accurate results are required. It is, however, prudent to stretch the grid towards the domain boundaries to reduce simulation time and computer memory requirements.

• 3.5.12    Information

The Information command displays status information about the defined grid, while the List command lists the grid coordinates in the working direction.

• 3.5.13    List

The Information command displays status information about the defined grid, while the List command lists the grid coordinates in the working direction.

• 3.5.14    Display

Three mutually exclusive options are available in the Display menu:

• •    Off: The grid is not displayed. Only the geometry is shown.

• •    Working Direction: The grid is displayed in the working direction only.

• •    All Directions: The grid is displayed in all three directions.

• 3.5.15    Select

The selected region includes grid planes between the planes that are selected as the lower and upper limits. If only one plane is selected, the upper and lower limits are the same grid plane. Grid planes are selected using the following commands:

• •    Lower boundary

– Select the next grid plane: CTRL+RIGHT

– Select the previous grid plane: CTRL+LEFT

• •    Upper boundary

– Select the next grid plane: CTRL+UP

– Select the previous grid plane: CTRL+DOWN

• 3.5.16    Grid-related operations
  
  3.5.17    Importing the grid from another job

Use the Import command in the File menu to import the grid from another job.

If a grid file name is entered in the command input field, the path must be encapsulated in apostrophes, for example:

∗ import "./cg000000.dat3"

If the command is selected from the menu bar, or if no name is specified in the command input field, the Import dialog box is displayed and the path and file name for a grid file can be be entered. A dialogue confirms that the current grid should be overwritten by the grid from the specified file.

• 3.5.18    Saving the grid

The Save and Save as commands in the File menu save the grid, together with the rest of the job data. Porosities must be recalculated following any change to the grid.

• 3.5.19    Grid-related utilities

FLACS-CFD is delivered with a command line tool, gm for creating and manipulating the grid. This tool can be used to quickly edit or obtain information about the grid.

• 3.6    Porosities menu

The Porosities menu contains commands for calculating and verifying porosities.

Calculate starts the porosity calculation program, FGC (Flacs Geometry Calculator).

Verify starts Flowvis in porosity verification mode.

• 3.6.1    Calculate

The Calculate command starts the porosity calculation program FGC.

Settings for FGC can be selected in the Preferences dialog in CASD.

• 3.6.2    Verify

The Verify command lets you view the calculated porosities. Flowvis is started for porosity verification. A 2D Cut Plane plot for the appropriate job is automatically created with volume and area porosities shown. The Plot Domain dialog box pops up. This dialog box lets you select other planes as wished.

By clicking inside a control volume, you can verify the porosity values for that volume.

• 3.7    Scenario menu

The purpose of this chapter is to outline how to edit the scenario sections. A short description of each section and the impact on the FLACS-CFD simulations will be given. The scenario file (cs-file) is an ASCII file and it is easy to edit manually as well as using CASD.

The scenario input is done in a scenario panel where sections can be expanded and collapsed. When a section has been expanded, the items in the section are displayed as a list. The method for editing a scenario section depends on the type of section.

Note:

Some advanced options and parameters are hidden by default. These can be shown by right clicking with the mouse and checking Show advanced.

Sections such as INITIAL CONDITIONS and IGNITION contain a list of parameters, each with one or more values. A parameter is selected for editing by double clicking on it or hitting the enter key. The scenario input can be done using the keyboard only with a combination of the arrow keys and the enter key.

Sections such as SINGLE FIELD SCALAR TIME OUTPUT and SINGLE FIELD _ 3D OUTPUT contain a list of items, which can be selected.

For some sections, each item has a subsection. For SINGLE FIELD SCALAR TIME OUTPUT you must select from a list of monitor points for each variable selected. An item is selected by clicking on it. To select several items using the mouse apply CTRL or SHIFT keys. If a selected option shall be deselected without selecting an alternative option, deselect by clicking while pressing the CTRL key.

Importing the scenario from another job

Use the Import command in the File menu menu to import the scenario from another job. You will be asked to verify that the current scenario is overwritten by the scenario from the specified file.

Saving the scenario

The Save and Save as commands in the File menu menu saves the scenario (together with the rest of the job data).

• 3.7.1    Scenario menu undo/redo

The scenario menu supports undoing and redoing most actions. As a general rule all actions except the Automatic grid refinement plugin support undo/redo.

Undoing is achieved by having focus on the scenario menu and using the CTRL+Z shortcut. Redoing is triggered by using the CTRL+Y shortcut.

There are also two buttons in the toolbar that can be used to trigger undo/redo in the scenario menu. See the screenshot below where these buttons are highlighted.

Figure 3.17: Undo/redo buttons for scenario menu

• 3.7.2    Scenario settings

  • 3.7.2.1    Simulation type

The following simulation types are available in CASD:

• •    Dispersion and ventilation

• •    Gas explosion

• •    Dust explosion

• •    Fire

• •    Inert

• •    Blast

• •    Pool

Note:

In FLACS-CFD 21.2 the simulation type Gas explosion (DDT) has been removed. This functionality is covered by the Gas explosion simulation type. Opening old scenarios that use the Gas explosion (DDT) simulation type is still supported in CASD and FLACS-CFD.

• 3.7.2.2    Write all variables

Enabling this option will write all available variables available in the current simulation type to the SINGLE FIELD VARIABLES section of the scenario file. Note that this only concerns variable definitions and does not automatically lead to output being written; see the sections regarding monitor points, pressure relief panels, and 3D output for how to obtain data for the variables.

• 3.7.2.3    cs-file compatibility

This option can be changed to produce scenario files that are compatible with different versions of FLACS-CFD, and will also impact which simulator and porosity calculator is selected when starting simulations using RunManager and runflacs.

Note:

This option is hidden by default. To make it available, right click in the Scenario settings window and check the Show advanced option.

• 3.7.2.4    Tags

This field is mainly used by FLACS-Risk to assign key-value pairs to scenarios, to support grouping in the post-processing. The input must be a comma-separated string, such as Geometry=BangBox, Wind=0/5.

• 3.7.2.5    Frequency

The frequency field is used by FLACS-Risk projects to assign a frequency to each scenario. The frequency is used in post-processing to generate exceedance curves.

• 3.7.3    Monitor points

Monitor points are user-defined locations in the simulation domain where one or more variables are to be monitored during the simulation. The maximum number of monitor points allowed is currently 8000. Positions for monitor points are given in the unit selected in Options Preferences (normally meter) For the fire simulation type, monitor points additionally need to be assigned a direction along which the incident radiative flux is calculated. The monitor point direction is specified as a vector. If the direction is not specified then the maximum value will be output.

Output variables to be written for a monitor point are selected by editing the monitor point. Several monitor points can be edited at the same time by marking them and clicking 'Edit'.

FLACS-CFD identifies the eight surrounding Control Volume (CV) centres and writes an interpolated value of the specified variables to the scalar-time output file (nodes on the other side of a wall or with zero porosity will not be used when interpolating). Here the eight surrounding CV centres define the corners of a parallelepiped used during the interpolation (for a uniform grid with the same CV length in all three axis directions this parallelepiped will be a cube). When a monitor point is located in the centre of a Control Volume (CV) and output is given for a scalar variable (e.g. pressure) stored during the simulation at the central nodes of the numerical grid (the CV centres), then the value reported as output for the scalar variable is the same as the value at the CV centre itself (except for a possible very small difference due to numerical rounding errors).

Attention:

Monitor points should not be placed in the same grid cell as a solid wall unless the wall is thicker than a single grid cell. Usually it is best to enter monitor points according to the grid, not according to the geometry. During the porosity calculations, walls are adjusted to the nearest control volume face (grid line), which can result in a monitor point that was positioned on one side of a wall now being on the other side of the wall! So, if monitor points are placed on opposite sides of a solid wall, then it is possible that they will be considered in FLACS-CFD to be on the same side of the wall (unless the wall is thicker than a single grid cell). Also ensure that no monitor points are inside fully blocked control volumes. For FLACS-Blast simulations, monitor points should not be in cells with porosity ≤ 0.5, see the bast section in Modelling and application limitations.

Figure 3.18: Specification of monitor points

NO!               YES

GRID LINES

■ WALLS
+ MONITOR POINT LOCATIONS

Figure 3.19: How to position the monitor points

See also:

Monitor points can be added quickly using the Arrange items functionality.

How to obtain output for flow variables at monitor points is described in the section on

Single field scalar time output below.

• 3.7.3.1    Naming monitor points

Monitor points are given the generic name MP # upon creation. The # is replaced by sequential numbering (”1”, ”2”, ”3”, etc.), converting the generic names into ”MP 1”, ”MP 2”, ”MP 3”, etc. The sequential

numbering is kept consecutive, so that if monitor points in the middle of the list is deleted, monitor points with higher numbers will be renamed, i.e. assigned new numbers to close the gaps in the numbering. Monitor points can be given custom names, and such names will not be affected by the automatic numbering, unless they include a #.

• •    It is possible to give multiple monitor points the same custom name, but this should be avoided as it may lead to confusion later when plotting results.

• •    Using a custom name that match a generic name (e.g. ”MP 5”) is also allowed, but may lead to multiple monitor points with identical names.

• •    The monitor points are stored internally in an ordered list, and new monitor points are added to the end of this list. The order (index) of the monitor points in this list is fixed, and is not changed when renaming or deleting monitor points.

• •    The sequential numbering for monitor points with names containing a ”#” is computed by finding the next unused consecutive number when iterating through the internal list. This means that when renaming a monitor point from e.g. ”MP #” to ”INSTRUMENT #”, the new name will contain the same number as before, but the visual position of the monitor point in the list may change due to sorting.

• •    The visual order of monitor points in the scenario menu is controlled by the chosen sorting criteria, independent of the internal list position (index).

• 3.7.3.2    Grouping of monitor points

Groups can be defined to organise monitor points. All grouping functionality is available in the context menu, which can be accessed by right-clicking in the monitor points section of the scenario menu. The list of monitor points in a group can be collapsed by double-clicking on the group name; another double-click will expand the list again. When marked, one or several monitor points can be dragged into, between or out of a group. Each monitor point can be assigned to maximally one group. See the picture below for an example.

• 3.7.3.3    Labels for monitor points

Aside from organising monitor points in groups, they can also be assigned one or several labels. Labels can be exploited by filtering the list of monitor points to show only those that have one (or several) specified labels. See the picture below for an example. The label and filtering functionality is accessed by right-clicking in the monitor points section of the scenario menu.

Figure 3.20: The monitor points in this example have been assigned to two groups representing the decks of a module. Additionally, labels have been assigned, and a filter is active so that only those monitor points that have the label Gas detector are shown.

• 3.7.4    Pressure relief panels

Pressure relief panels are commonly used in the process industry as a mitigating device in the case of an explosion. When the pressure forces on the panel exceed a certain limit, the panel yields and the pressure is relieved. In FLACS-CFD, special planar elements inside the simulation volume are used to model the effect of explosion relief panels and yielding walls. They are specified as boxes where one, and only one, of the three side lengths must be zero. In addition, several parameters such as the yield pressures, area porosities and drag factor may be specified.

A panel may be active or passive. An active panel will initially modify the porosity in the region it covers, and again when the pressure difference over the panel exceeds the given limit. If the initial porosity is set to 0 and the final porosity is set to 1 the panel will start as being closed and end up as being open. This is how the behaviour of a real yielding panel is emulated. A passive panel will never modify the porosity, but it may be used to monitor the same data as an active panel. The maximum number of panels allowed is currently 8000. There are 5 different active panel types in standard FLACS-CFD (and additional 2 in flacscfd):

Table 3.21: Panel types in FLACS-CFD

The edges of a panel are automatically adjusted to the closest grid line. Specify panels whose dimensions match the grid, either by adjusting the grid or by modifying the panel (see Summary of grid recommendations ).

One topic that needs special attention is the presence of solid structures close to the panel area. For example structural beams may constitute quite large blockages that must be accounted for, especially since they also occur at the vent openings of typical offshore modules. In such cases the panel area must be defined using several panels with solid beams in between. Smaller beams, often an integral part of the support frame of the pressure relief panels, may be accounted for by adjusting the final panel porosity for the panel itself. Apart from the abovementioned types of pressure relief panels, FLACS-CFD supports inactive panels. An inactive panel can be used to monitor variables, e.g. to measure average pressure on surfaces such as decks and walls. See the description of inactive panels.

If several panels are specified, they must not overlap each other anywhere, otherwise the behaviour is undefined; inactive panels are an exception and may overlap.

For panels, the same functionality for defining and using groups and labels is available as for monitor points. The full list of parameters from the scenario file is shown below. The type of the panel determines which of these parameters are relevant.

The parameters for specifying panel properties are described in the following sections.

• 3.7.4.1    Name

A textual, user-defined name or tag for the panel. The name is saved in the cs-file but not used by the simulator.

• 3.7.4.2    Insert

Integer identifying the panel.

• 3.7.4.3    Position

Cartesian coordinates [m] of the corner of the panel (the corner with lowest value of the coordinate in each axis direction).

• 3.7.4.4    Size

The panel is assumed to be a plane of rectangular shape. The dimension [m] in each of the axis directions is given. One dimension should be zero, this shows how the panel is oriented. If e.g. the dimension in x-direction is zero, the normal of the panel points in the x-direction. The other two dimensions should be positive. The panel edges and the position will be adjusted to match the grid lines perfectly in the FLACS-CFD code, so it is advised that you only specify panels which coincide with the grid lines, in order to avoid any confusion concerning the geometrical representation of the panel.

• 3.7.4.5    Material

For panels, the materials defined in the CASD database may be assigned, but they will not lead to the use of the associated colour. To change the colour of a panel, the colour has to be given as hue value and must be the only value provided to the MATERIAL property, for example

MATERIAL                        "300"

in the cs-file or by clicking Edit in the Pressure relief panels section of the scenario menu in CASD.

• 3.7.4.6    Panel type

The current section describes the eight different panel types: INACTIVE (the only passive panel type), UNSPECIFIED, POPOUT, HINGED, POPOUT RIGID, HINGED RIGID, PLASTIC, and OVERLAY.

• 3.7.4.6.1    Inactive panel A passive panel does not affect the numerical simulation in any respect (neither the geometrical description, including the porosities, nor the flow field), it is only included to monitor variables related to the area which the passive panel occupies (e.g. area-averaged pressure over all the control-volume faces of the panel). Only the parameters INSERT, POSITION, SIZE, and MATERIAL are relevant when the PANEL TYPE is INACTIVE (in CASD). In the cs-file, a panel is marked as inactive by removing the PANEL TYPE line in the panel definition. INACTIVE panels are available under Single field scalar time output in the Scenario menu.

• 3.7.4.6.2    Unspecified, Popout and Hinged panel An active panel (all panel types except INACTIVE) will generally affect both the porosities representing the geometry and the flow field. For the active panels both an initial and a final area porosity value is given (open area divided by total area). The initial porosity corresponds to the state of the panel before it has started to yield due to external pressure forces. The final porosity corresponds to the state of the panel after it has yielded completely due to pressure forces.

Each control-volume face covered by the panel is treated separately. Thus it is possible, depending on the scenario, that one part of the panel is open, while at the same time other parts are closed.

The way of using the initial and final porosities in the FLACS-CFD code depends on the type of panel considered. In the case of the panel types UNSPECIFIED, POPOUT, and HINGED, for each control-volume face that is covered by the panel, the porosity representing the panel is also the porosity of the control-volume face, regardless of any other equipment or structure included in the geometry.

• 3.7.4.6.3    Popout rigid and Hinged rigid panel POPOUT RIGID and HINGED RIGID panels can be considered to be the more accurate models of POPOUT and HINGED panels (note, validation of the rigid panel type is still ongoing), and is different in the way the area porosity of each control-volume face initially covered by the panel is evaluated. Panel's average area porosity and traveled distance (or opening angle), is updated based on forces and torques acting on the total panel area as it is assumed to be rigid. In case of POPOUT RIGID panels, area porosities of individual control-volume faces are equal to the average panel area porosity, whereas in case of HINGED RIGID panels they depend on face's relative distance to hinges. Hinges position of HINGED RIGID panels must be specified in HINGES. Additionally, for this panel type the user may specify side outflow planes - SIDE OUTFLOW.

The opening angle or the traveled distance of the panel can be visualized in Flowvis or accessed through Python API when PTRA variable is selected in the SINGLE FIELD SCALAR TIME OUTPUT. The value of PTRA is signed and is positive for translations in the positive axis direction and rotations in the positive direction about the hinge axis.

• 3.7.4.6.4    Overlay and Plastic panel A panel of type OVERLAY is superimposed on other equipment. For an OVERLAY panel, the value of the area porosity determined by the panel is multiplied by the value of the area porosity determined by other geometrical objects (in the absence of any panel) giving the effective area porosity, for each control-volume face covered by the panel. Let us consider an example where the final porosity of the panel is 1 (fully open). After the panel has yielded completely for all the control-volume faces covered by the panel, the area porosities have the same values that they would have if no panel was included in the geometry. So in this case other geometrical objects than the panel itself can not “blow out” together with the yielding panel (cf. the comments above).

The panel type PLASTIC emulates a plastic sheet (commonly used in experiments). For a PLASTIC panel, in case of initial area-porosity, for each control-volume face which is covered by the panel, the porosity representing the panel is also the porosity of the control-volume face, regardless of any other equipment or structure included in the geometry (as in the case of the panel types UNSPECIFIED, POPOUT, and HINGED). Usually the initial area-porosity of a PLASTIC panel is zero (completely blocked). If the PLASTIC panel has yielded completely, the area porosities have the same values that they would have if no panel was included in the geometry (as in the case of an OVERLAY panel with final area-porosity 1). For a PLASTIC panel the final area-porosity is always assumed to be 1, regardless of the user-given value.

Panels of the types PLASTIC or OVERLAY are assumed to be light panels, and inertial forces are neglected by the FLACS-CFD code during the dynamical process when the panel yields due to pressure forces. In the case of panels of types UNSPECIFIED, POPOUT, or HINGED, inertial forces are in general taken into account.

• 3.7.4.6.5    The +IMP panel types The standard panel types will yield at a given negative or positive pressure. In some situations it can be necessary for panels to also take into account the pressure impulse. To activate this, add the suffix +IMP to the end of the panel type string, e.g

PANEL_TYPE POPOUT+IMP

OPENING_PRESSURE_DIFFERENCES 0.05 0.005 (bar bar*s)

When using this the input to OPENING PRESSURE DIFFERENCES changes to

• •    Parameter 1 is yield pressure for both negative and positive direction [bar]

• •    Parameter 2 is yield pressure impulse both negative and positive direction [bar∗s]

The panel will yield if both the pressure and pressure impulse yield values are exceeded.

This is valid for panel types HINGED and POPOUT.

• 3.7.4.7    Opening pressure differences

When the net pressure over the panel (pressure on the negative side relative the coordinate axis minus pressure on the positive side, i.e. the net pressure from the fluid acting on the panel) exceeds the given limits, the panel starts to yield. Two opening pressure-differences, in units of [bar], have to be given by the user, the first corresponds to the case when the net pressure acts in negative direction, the second when the net pressure acts in positive direction. If for example the OPENING PRESSURE DIFFERENCES are given by -0.1 and 0.2, the panel starts to yield when the net pressure is less than -0.1bar (negative direction) or greater than 0.2 bar (positive direction). Notably, the FLACS-CFD simulator disregards the sign of the user-defined opening pressure-differences. Hence, if the OPENING PRESSURE DIFFERENCES were given instead by 0.1 and 0.2, or by 0.1 and -0.2, the effect on the numerical simulation would be exactly the same. The opening pressure-differences must be given for the active panels (all the panel types accept INACTIVE).

• 3.7.4.8    Initial and final porosity

The initial area porosity [-] of the panel (open area divided by total area) corresponds to the state of the panel before it has started to yield due to external pressure forces. Similarly the final porosity corresponds to the state of the panel when it has yielded completely. In the case of a PLASTIC panel, the final area-porosity should be set to 1 in order to correspond to how the FLACS-CFD code works (the final area-porosity is always assumed by FLACS-CFD to be 1, regardless of the given value). How FLACS-CFD uses the initial and final porosities depends on the type of panel considered, see above. The initial and final porosity must be given for the active panels (all the panel types accept INACTIVE). The value of the porosity range from 0 (totally blocked) to 1 (fully open). It is expected that the initial porosity is less than the final porosity (the net pressure opens up the panel). If this is not the case, the FLACS-CFD code gives a warning.

After the panel has started to yield, the effective area porosity will gradually change as function of time until the panel has yielded completely. How long time it takes before the panel has yielded completely depend on the pressure forces acting on the panel, the weight of the panel, and the type of panel (for example will the dynamics when a HINGED panel opens, be somewhat different from the dynamics when a POPOUT panel opens). The panel average porosity PPOR may be monitored as function of time giving some information about the yielding process, confer the description of PPOR .

• 3.7.4.9    Weight

The parameter WEIGHT is relevant for the panel types POPOUT, POPOUT RIGID,HINGED, and HINGED RIGID. This parameter is defined as the mass per unit area of the part of the panel that is moved when the net pressure acting on the panel exceeds the given opening pressure-difference; (mass of moved area of panel)/(moved area of panel) [kg/m²]. The denominator (moved area of panel) is not the total area, but only the area of the moved part of the panel (in general this is less than the total area). The dynamics when the panel yields and part of the panel is accelerated and move away from its initial position, is modelled in the FLACS-CFD code. When specifying a panel type that includes the WEIGHT parameter, the inertial forces must be there when the panel yields. This means that value of WEIGHT should be set to a positive number greater than zero, or the FLACS-CFD simulator will terminate with an error message in the log file. It is only the part of the panel that is accelerated and moves away from its initial position that should contribute to the mass of the moved area of the panel. The mass of a rigid frame that does not yield, should not be included.

Let us consider an example with a POPOUT pressure relief panel: Uniform steel plates with mass per unit area 10kg/m² are mounted on a strong frame. When the pressure difference exceeds a certain level, the steel plates pop out and move away from the frame. The final porosity corresponds to the state when the panel has yielded completely (the steel plates have moved sufficiently away). Depending on the structure of the strong frame (assumed not yielding), the final porosity could e.g. be 0.9. And in this example the parameter WEIGHT is given as input 10kg/m² (the value 10kg/m² is within the typical range of values for WEIGHT for pressure relief panels used at offshore installations).

• 3.7.4.10    Drag coefficient

A dimensionless drag-coefficient [-] has to be given for the panel type UNSPECIFIED (for the other panel types it is not relevant to specify this parameter). The drag coefficient is used when the drag force from the panel on the fluid is modelled (both before, during, and after the panel has yielded). The value of the DRAG COEFFICIENT is zero or positive. A typical value is 2.0 (the value 2.0 is set by the FLACS-CFD code as a fixed preset value for the panel types POPOUT and HINGED).

• 3.7.4.11    Maximum travel distance

The maximum travel-distance [m] has to be given for the panel type UNSPECIFIED (not relevant for the other panel types). The use of the maximum travel-distance is based on a rough approximation. The maximum travel- distance is the smallest distance from the initial position of the panel to the position where the yielded panel no longer affects significantly the effective area-porosity at the initial position of the panel. The maximum travel-distance is used to model the effective area-porosity at the initial position of the panel during the dynamical process when the panel yields. A typical value of the MAXIMUM TRAVEL DISTANCE is in the order of 1m (for the panel types POPOUT and HINGED there is an in-built model in the FLACS-CFD code for the effective area-porosity that does not need an input value of the MAXIMUM TRAVEL DISTANCE). You do not need to explicitly specify the maximum travel distance [m] for a POPOUT or HINGED panel. For a POPOUT panel, the maximum travel distance dmax [m] (i.e. the panel displacement after yielding, where the panel frame is fully open, corresponding to the final porosity) is calculated from the sub-panel width w [m] and the sub-panel height h [m] according to the formula:

Here the width w is the first panel subsize, and the height h is the second panel subsize (see below). For example, if the panel subsizes are specified as 'PANEL SUBSIZES 2.0 1.0', then the width is 2.0 metres and the height is 1.0 metre.

A POPOUT panel covers a certain number of Control Volume (CV) faces for the given numerical grid. As a simplification (or model limitation), the panel displacement at each CV face is assumed to be independent of the other CV faces. The force acting at each CV face is F = A dp [N], where A [m2] is the effective area and dp [Pa] is the local pressure difference (drag forces are also accounted for). The velocity and displacement at each CV face is updated for every time step. The acceleration a [m/s²] is calculated as a = F/m where m [kg] is the mass of the segment of the yielding panel that covers the CV face. Integrating the acceleration a with respect to time gives the velocity v, and integrating the velocity v over time gives the panel displacement d as function of time after yielding. The area porosity at each CV face covered by the POPOUT panel will change linearly from the specified initial porosity to the specified final porosity as the panel moves from zero to the maximum travel distance.

• 3.7.4.12    Panel sub-sizes

The parameter PANEL SUBSIZES has to be defined for the panel types POPOUT or HINGED (not relevant for the other panel types). These panel types are assumed to consist of sub-panels mounted on a frame. The width [m] and the height [m] of the sub-panels need to be given (it is assumed in the numerical model that all the sub-panels are of uniform size). Both the width and the height should be larger than zero. In the case of the panel type HINGED it is assumed that each sub-panel turns on a hinge when it yields. The width of the sub-panel is defined as the dimension in the direction normal to the axis of the hinge. It is important (since it affects the model in FLACS-CFD) to specify the width of a HINGED panel first and then the height, in the parameter PANEL SUBSIZES (for a POPOUT panel it is of no importance which dimension that is defined as the width).

See also:

Panels can be added quickly using the Arrange items functionality.

How to obtain output of flow variables on panels is described in the section on Single field scalar time output below.

• 3.7.4.13    Hinges (flacscfd only)

The location of the hinges can be specified only for HINGED RIGID panels. Parameter HINGES takes one of the values denoting hinges axis position with respect to the panel. For instance for the XY panels the following values are allowed: +X, -X, +Y, -Y.

• 3.7.4.14    Side outflow (flacscfd only)

Side outflow can be specified for HINGED RIGID panels. By default (None) the model uses the most conservative approach, where only the projected panel opening area is taken into account in average panel porosity calculations. The user may change this behaviour and select also Frontal , Lateral or both areas. Taking into account both areas is the most accurate modelling approach for panels, assuming their corresponding areas are free and do not interfere with neighbouring panels. When in doubt, it is recommended to use the most conservative approach (with the smallest opening area).

• 3.7.4.15    Using panels in fire simulations

All panel types, including pressure relief panels, are supported by the FLACS-Fire solver. The DTM radiation calculations will capture any changes to panel porosity during the simulations (e.g. due to panels failing or when using an event file).

• 3.7.5    Single field scalar time output

Rather than having its own entry in the scenario menu, the output of values at monitor points and panels is selected directly when defining the monitor point or panel in their respective scenario menu sections. One or several variables can be selected and deselected by left-clicking or dragging, respectively. Typically the same set of variables should be measured at all monitoring locations. This can be done quickly by selecting all monitor points/panels, right-clicking and selecting 'Edit' on the context menu. The variables can then be selected for all selected monitor points/panels.

An example of how the single field scalar time output selection translates to the corresponding section in the scenario file is shown below. Here NP identifies the variable P (pressure) whereas NPP selects the variable PP (panel pressure), which gives the average pressure across a the surface of a panel:

SINGLE_FIELD_SCALAR_TIME_OUTPUT

NP 1 2 3 4 5

NPP 1 2 3

This shows that pressure is reported for monitor points 1-5 and panel pressure is reported for panels 1-3. The most commonly used monitor point variables for explosion simulations are pressure (P), dynamic pressure (DRAG), panel pressure (PP), pressure impulse (P IMP) and sometimes flow velocity (UVW). For dispersion calculations volume gas concentration (FMOLE) and flow velocity (UVW) are often used.

The monitor point results for job 010100 are written to the r1010100.dat3 file which is read by Flowvis. If ASCII data is required, the r1file-utility program can be used (see the section on FLACS-CFD utilities).

The first section in the scenario file defines the names and identifiers for all variables which may be selected for output from FLACS-CFD. To select alternative units for certain variables (e.g. psi or kPa for pressure or K for temperature) the scenario file should be edited manually. The variable pressure is described in the scenario file as follows:

NP        "P        " 1 "(barg)            "  N  "Pressure"

The output can be obtained in a different unit (psig) can be obtained by editing this as follows:

NP        "P        " 1 "(psig)            "  N  "Pressure"

Similar changes can be made for other variables and other units. Notably the unit of time must always be seconds in the scenario file. After running a simulation, it is possible to change the unit of time as well as other units in Flowvis.

A complete list of all variables available can be found in section Output variables in FLACS-CFD.

• 3.7.6    Single field 3D output

This is an output facility in FLACS-CFD which makes it possible to generate plots of the spatial distribution of the variables (e.g. cut plane plots and volume plots) at different moments in time. Before running a simulation, the user needs to specify the list of desired variables for SINGLE FIELD 3D OUTPUT, an example from scenario file is shown below (here P, PROD and VVEC are selected in CASD):

SINGLE_FIELD_3D_OUTPUT

NP

NPROD

NVVEC

NU

NV

NW

When velocity vectors are selected for output (VVEC), the velocity components U, V and W will automatically be selected. These must not be deselected while VVEC remains selected (this might, for example, happen when editing the scenario file manually). Failure to keep the result file and the scenario file consistent will lead to strange results shown in Flowvis.

This type of output may give very large files (r3-files). If you want to save disk space, the number of output variables and the number of time instants for output must be limited. The r3-files are binary, if ASCII data is wanted the utility program r3file can be applied.

The most commonly used variables for explosion modelling are pressure (P), flame (PROD), sometimes gas volume concentration (FMOLE), dynamic pressure (DRAG), maximum pressure (P MAX) and velocity vectors (VVEC). For dispersion FMOLE and VVEC will be the most common variables to report.

In certain situations the variable P MAX may not be written to even if specified (zero results everywhere). This may happen if the simulation job requires more RAM than allowed (e.g. due to self-defined limits in Linux)

To specify output times DTPLOT and NPLOT will normally be used (see Simulation and output control section), and sometimes also cc-files (see Runtime simulation control file section). To create animations it is normally recommended to have plots at 100-200 different moments in time. When creating results files to be used for animations a combination of DTPLOT and NPLOT is usually recommended for explosions, for dispersion only DTPLOT should be used (i.e. keep NPLOT=-1).

Units of output variables can be changed using the technique described in the previous section.

A complete list of all variables available can be found in section Output variables in FLACS-CFD.

• 3.7.7    Setup

This section of the scenario menu has to be enabled manually and allows to specify the advanced settings that can be provided for a simulation with the help of a setup file. The setup file written by CASD will have the name cs<jobno>.SETUP and will be read automatically by the Flacs simulator unless a setup file (with a different name) is specified explicitly on the command line call to Flacs.

• 3.7.8    Simulation and output control

This section describes parameters for general simulation and output control. The settings entered into the scenario file by default for gas explosion simulations are listed below:

Maximum time-1

Last timestep-1

CFLC5

CFLV0.5

MODD1

NPLOT-1

DTPLOT-1

When using flacscfd, the following parameter is also available:

Solver mode

Enable DDT detection

Force DDT at time

When Solver mode is set to STEADY, the following parameters are also available:

UNDERRELAX_P

UNDERRELAX_UVW

CHECK_CONVERGENCE

CONVERGENCE_TOLERANCE_P

CONVERGENCE_TOLERANCE_FUEL

CONVERGENCE_TOLERANCE_FLAMMASS 0.001

CONVERGENCE_TOLERANCE_FUELMASS 0.001

CONVERGENCE_TOLERANCE_FUELRATE 0.001

CONVERGENCE_TOLERANCE_MASSRATE 0

CONVERGENCE_TOLERANCE_VELMAX 0.0001

If Show advanced is checked, the following parameters are also available:

Start time-1

Minimum time-1

Load number-1

Load job name""

Timestep code""

Special control keys""

INCOMPRESSIBLE0

WALLF1

HEAT_SWITCH0

For dispersion simulations, higher values (20 and 2) are recommended for the CFL numbers. NPLOT should be -1 and a finite value of DTPLOT should be given.

A detailed description of each parameter is given below.

• 3.7.8.1    Start time (TSTART)

Note:

Only available if Show advanced is checked.

The value entered for Start time is saved in the scenario file as TSTART. This variable makes it possible to specify a start time for simulation (-1 means not applied => default is zero or time of dump-file). If a dump-file exists, one can still adjust Start time, but the previous history of the simulation cannot then be stored using the KEEP OUTPUT option in a setup file.

• 3.7.8.2    Minimum time (TMIN)

Note:

Only available if Show advanced is checked.

The value entered for Minimum time is saved in the scenario file as TMIN. This variable makes it possible to define a minimum time for the simulation. When TMIN is set to a positive number, the automatic stop criteria will not activate before the physical time has reached the value of TMIN. This can be useful for blast simulations.

If TMIN is set to -1, then TMIN will not affect the activation of the automatic stop criteria. However, whether TMIN is defined at all, or is set to -1, will in general affect whether FLACS-CFD runs until the value of TMAX (Maximum time) is reached or stops earlier, at a physical time less than TMAX.

Note:

The automatic stop criteria are disabled in the FLACS-Fire solver, so setting TMIN has no effect for these simulations.

See also:

The section on Maximum time contains further information and some examples.

• 3.7.8.3    Maximum time (TMAX)

The value entered for Maximum time is saved in the scenario file as TMAX. This is the maximum time interval (seconds) that the simulation will last. The default value of -1 is generally appropriate for explosions simulations. Setting TMAX=-1 means that no maximum time is specified, and the automatic stop criteria will be applied. The automatic stop criteria work well for most explosion calculations. A simulation will be stopped automatically when ignition has happened and one of the following criteria are met:

• •    at least 90 % of the fuel has been burnt or left the domain, or

• •    at least 50 % of the fuel has been burnt or left the domain and the average pressure becomes negative

As soon as one of these criteria is fulfilled, the remaining time to be simulated is taken to be 20 % of the time that has passed since the ignition in the simulation. After this time the simulation will stop automatically.

There are no automatic stop criteria for dispersion and fire simulations, and so these will run indefinitely (until manually killed by the user) if Maximum time is set to -1 for these scenarios.

Automatic stop criteria may not be useful for all explosion scenarios. If far-field blast pressures are of interest, the automatic stop criteria should not be used as they may stop the simulation before blast waves have hit their target.

In a gas dispersion or fire simulation, an appropriate TMAX will typically be from a few seconds to a few minutes. Simulation results are not affected when varying this parameter.

When TMIN (Minimum time) is not specified in the scenario file, and TMAX is set to a positive value less than 10 000, then FLACS-CFD will not stop due to the automatic stop criteria, but will run (whenever possible) until the physical time reaches the value of TMAX.

However, when the TMIN is specified in the scenario file, (even when TMIN=-1), then FLACS-CFD may stop before the physical time reaches TMAX (provided that TMAX is set to a positive value larger than TMIN but less than 10 000). If TMIN is set to a positive value larger than the time determined by the automatic stop criteria, then FLACS-CFD will run (whenever possible) until the time reaches the value TMIN and then stop the simulation. If TMIN is set to a value less than the time of the automatic stop criteria, then FLACS-CFD will run (whenever possible) until the automatic stop criteria are met.

Some examples of different Minimum time and Maximum time settings follow:

• 3.7.8.3.1    Example 1: Typical explosion simulation

Automatic stop criteria are used if the cs-file has these settings:

TMIN -1

TMAX -1

• 3.7.8.3.2    Example 2: Explosion simulation with points of interest in the medium/far field

In such cases, use STEP="KEEP LOW" to keep the time step small after the explosion and to prevent smearing of the pressure waves (see Timestep code). Example cs-file setting are:

TMIN 3

TMAX -1

These settings will stop the simulation at 3 s unless more than 10 % of the fuel is still present. The appropriate TMIN (Minimum time) depends on the distance to the point of interest and the time of the explosion peak pressure.

• 3.7.8.3.3    Example 3: Dispersion or Fire simulation

By prescribing

TMIN -1

TMAX 100

the simulation will stop at 100 s.

• 3.7.8.4    Last timestep (LAST)

Note:

Only available if Show advanced is checked.

The value entered for Last timestep is saved in the scenario file as LAST. This stop criterion is based on the maximum number of iterations allowed for the simulation. The default value set by CASD is -1, which means that there is no limitation to the number of iterations. This parameter is particularly useful when the steady state solver is used. The dump snapshot is written automatically when the LAST iteration is reached and the simulator exits normally.

• 3.7.8.5    Load number (LOAD)

Note:

Only available if Show advanced is checked.

The number entered for Load number is saved in the scenario file as LOAD. This setting makes it possible to load a dump snapshot from a file (either from the CGNS file or the rd-file). It is equivalent to legacy option NLOAD in the cc-file. The default value set by CASD is -1, which means that no snapshot will be loaded. Otherwise, the dump snapshot denoted by LOAD will be loaded. If LOAD is set to 0, then the simulator will load the last available dump snapshot.

• 3.7.8.5.1    Example 1 - load snaphot #2 into simulation 000000

Load number setting in the cs-file:

LOAD 2

What happens:

• 1.    Simulator first tries to read ”rd000000.n002”, which is an obsolete Flacs2 dump file containing snapshot #2.

• 2.    If no rd-file file is found and the simulator is Flacs2, then the simulator will exit with an error message.

• 3.    If no rd-file file is found and the simulator is Flacs3, then the simulator tries to read dump snapshot #2 from the CGNS file ”000000.cgns”.

• 4.    If any of the files are read, then the simulator restores the exact conditions from the time when the file was written.

• 5.    Simulation output is appended to the existing result files.

• 6.    An error message is given if neither ”rd000000.n002” nor the CGNS file exist.

• 3.7.8.5.2    Example 2 - load the last available dump snapshot from the CGNS file into simulation 000000

Load number setting in the cs-file:

LOAD 0

What happens:

• 1.    The last available dump snapshot from the CGNS file ”000000.cgns” is read at simulation startup, restoring the exact conditions from the time when the file was written.

• 2.    Simulation output is appended to the existing result files.

• 3.    An error message is given if the CGNS file does not exist.

• 3.7.8.6    Load job name (JLOAD)

Note:

Only available if Show advanced is checked in flacscfd.

The string entered for Load job name is saved in the scenario file as JLOAD. This makes it possible to change the name of the CGNS file that the dump snapshot is loaded from. When JLOAD is specified in the cs-file, the simulator appends ".cgns" to the end of the provided string, and loads the dump snapshot from the cgns file that corresponds to the resulting filename. When JLOAD is not specified in the cs-file, the current job number is used.

Note:

When grids defined in the grid file differ from those in the CGNS file that contains the dump snapshots, the name of the CGNS file must be set to the string entered for JLOAD, and this must differ from the current job name.

If JLOAD is set, then the history of the simulation cannot be kept using KEEP OUTPUT in a setup file.

• 3.7.8.6.1    Example 1 - load from specified CGNS file into simulation 000000 and scale if necessary

LOAD and JLOAD settings in the cs-file:

LOAD 2

JLOAD "dispersion_results"

What happens:

• 1.    Dump snapshot #2 from the file ”dispersion results.cgns” is read at simulation startupn restoring the exact conditions from the time that the file was written.

• 2.    Results are projected onto the new grid if necessary.

• 3.    An error message is given if the file ”dispersion results.cgns” does not exist.

• 4.    A new CGNS results file, ”000000.cgns”, is created for the job and ”dispersion results.cgns” is not modified.

• 3.7.8.7    CFLC

This is a Courant-Friedrich-Levy number based on sound velocity. The value of CFLC connects the simulation time step length to the control volume size through signal propagation velocity (in this case the velocity of sound), in the following way:

Each time step length is chosen so that sound waves may propagate only a limited distance, which is the average control volume length multiplied by the value of CFLC. The default value set by CASD is CFLC=5 for explosion simulations. The time step limit imposed by this criterion is normally dominant in the early phase of an explosion, when flow velocities and combustion rate are still low (see also CFLV).

Simulation results may change with this parameter, and it is therefore not recommended to change its value for explosion simulations (since this would nullify Validation). If convergence problems occur (a rare occurrence), then CFLC may be reduced by a factor of 2. However, other problems should be ruled out first. Large changes to the CFL number (e.g., an order of magnitude) are never recommended for normal simulations.

For dispersion and ventilation simulations, the default value of CFLC=10 is recommended. This can be increased by the grid refinement factor (if applicable). If the grid is refined near the leak by a factor of 5, then using a CFLC number of 10∗5=50 may be considered (a lower value should be used in case of stability problems).

For fire simulations, the default value of CFLC=20 is recommended, however if stability issues are encountered then this can be halved to make the calculations more stable.

For far-field blast simulations, this should be combined with STEP="KEEP LOW" to keep the time step short, even after the explosion is outside the ”core” area, to reduce smearing of the pressure waves (more information is given Timestep code).

• 3.7.8.8    CFLV

This is a Courant-Friedrich-Levy number based on fluid flow velocity. The value of CFLV connects simulation time step length to control volume dimension through signal propagation velocity (in this case the fluid flow velocity), in the following way:

Each time step length is chosen so that the fluid may propagate only a limited distance, which is the average control volume size multiplied by the Courant number. The default value set by CASD is CFLC=0.5 for explosion simulations. The time step limit imposed by this criterion is normally dominant in the later phase of an explosion, when flow velocities and combustion rate are high (see also CFLC).

Simulation results may change with this parameter, and it is therefore not recommended to change its value for explosion simulations (since this would nullify Validation). In rare cases where convergence problems occur, then CFLV may be reduced by a factor of 2. However, other problems should be ruled out first. Large changes to the CFL number (e.g., an order of magnitude) are never recommended for normal simulations.

For dispersion and ventilation simulations, the default value of CFLV=1 is recommended, and for fire simulations, the default value of CFLV=2 is recommended. A lower value should be used in case of stability problems.

Some additional cosiderations are required when setting CFLV for the incompressible solver, these are detailed in Time step for the incompressible solver .

• 3.7.8.9    Solver mode (MODE)

Note:

Only available in flacscfd.

The value entered for Solver mode is saved in the scenario file as MODE. Solver mode is set to TRANSIENT by default which is the recommended setting for most simulations, especially these involving transient phenomena. If the solver mode is set to STEADY, the steady-state solver is activated. Steady-state solver switches off the CFL stability criterion in the time step determination and ignores the CFLC and CFLV settings. The steady-state solver ignores the TMAX (Maximum Time) stop criterion by default, and uses the convergence stop criteria if CHECK CONVERGENCE (Check convergence) is enabled. Additionally, the maximum number of iterations can be set using the LAST (Last timestep) stop criterion. FLACS-CFD writes the dump snapshot automatically on either convergence or reaching the Last timestep stop criterion.

Note:

Using the steady state solver, a steady state solution can be obtained in a fraction of time required for simulations in transient mode. However, in some cases the solution may diverge. This was observed in simulations involving high mass flow diffuse leaks.

• 3.7.8.10    Enable DDT detection (DDT)

Note:

Only available in flacscfd.

The value entered for Enable DDT detection is saved in the scenario file as DDT. The default value set by CASD is AUTO, which means that detonation will be triggered automatically for hydrogen explosions if DPDX (DPDX) is higher than 1. If Enable DDT detection is set to Off detonation will not be triggered. The time at which DDT is triggered can be modified using DDT TIME (Force DDT at time).

The detonation solver is an engineering approach to simulate detonations. When detonation is activated the maximum speed is allowed to exceed sonic speed and FLACS-CFD can represent supersonic flow. The time step is reduced by a factor of 5 and the burning velocity is set to a constant value.

In order to simulate detonation for other fuels than hydrogen, Enable DDT detection has to be set to On.

• 3.7.8.11    Force DDT at time (DDT _ TIME)

Note:

Only available in flacscfd.

The value entered for Force DDT at time is saved in the scenario file as DDT TIME. The default value set by CASD is -1, which means that the detonation solver will be triggered for hydrogen explosions when DPDX > 1. If a DDT TIME is specified, the detonation solver will be triggered independently of the DPDX value and the fuel used.

Some examples of different Enable DDT detection and Force DDT at time settings follow:

• 3.7.8.11.1    Example 1: Hydrogen explosion simulation with automatic trigger of detonation

Automatic trigger of detonation when DPDX exceeds 1 if the cs-file has these settings:

DDT "AUTO"

DDT_TIME -1

\pragraph DDTDDTTimeEx2 Example 2: Hydrogen explosion simulation with specific trigger of detonation

Automatic trigger of detonation when time exceeds 0.02 seconds if the cs-file has these settings:

DDT "AUTO"

DDT_TIME 0.02

• 3.7.8.11.2    Example 3: Non-hydrogen explosion simulation with automatic trigger of detonation

Automatic trigger of detonation when DPDX exceeds 1 if the cs-file has these settings:

DDT "On"

DDT_TIME -1

Note: Automatic trigger of detonation for non-hydrogen explosion scenarios is not recommended, since the DPDX threshold would be hightly conservative for some fuels (for instance, hydrocarbons).

• 3.7.8.11.3    Example 4: Non-hydrogen explosion simulation with specific trigger of detonation

Automatic trigger of detonation when time exceeds 0.02 seconds if the cs-file has these settings:

DDT "On"

DDT_TIME 0.02

• 3.7.8.12    Underrelaxation P and UVW (UNDERRELAX ∗)

Note:

Only available when Solver mode (MODE) is set to STEADY in flacscfd.

The values set for Underrelaxation P and UVW are saved in the scenario file as UNDERRELAX P and UNDERRELAX UVW, respectively. These two parameters set numerical underrelaxation factors for continuity and momentum equations. They should be left unchanged unless user experiences stability or convergence problems. The stabilising solution describes how UNDERRELAX P and UNDERRELAX UVW can be used to stabilize the solution.

• 3.7.8.13    Check convergence (CHECK _ CONVERGENCE)

Note:

Only available when Solver mode (MODE) is set to STEADY in flacscfd.

Enabling this setting by checking the box in CASD writes CHECK CONVERGENCE=1 to the cs-file. This activates a convergence stop criterion. By default, the criterion is enabled when the steady-state solver is used, and disabled when the transient solver is used. If the user sets CHECK CONVERGENCE=0 for a simulation using the steady-state solver, then only the LAST (Last timestep) stop criterion is used. The dump snapshot is written automatically on convergence and the simulator exits normally.

• 3.7.8.14    Convergence tolerance (CONVERGENCE TOLERANCE ∗)

Note:

Only available if CHECK CONVERGENCE (Check convergence) is enabled and MODE=STEADY (Solver mode) in flacscfd.

The value set for Convergence tolerance is saved in the scenario file as CONVERGENCE TOLERANCE_ ∗. Convergence tolerance can be defined for the following convergence criteria:

• •    CONVERGENCE TOLERANCE P - residual of the pressure correction (continuity) equation;

• •    CONVERGENCE TOLERANCE FUEL - residual of the fuel equation;

• •    CONVERGENCE _ TOLERANCE FLAMMASS - smoothed residual of the flammable mass in the default monitor region normalized by its maximum value;

• •    CONVERGENCE _ TOLERANCE FUELMASS - smoothed residual of the fuel mass in the default monitor region normalized by its maximum value;

• •    CONVERGENCE TOLERANCE FUELRATE - smoothed residual of the fuel rate in the default monitor region normalized by the leak rate (only checked if any leak found);

• •    CONVERGENCE TOLERANCE MASSRATE - smoothed residual of the mass rate in the default monitor region normalized by the leak rate (only checked if any leak found);

• •    CONVERGENCE TOLERANCE VELMAX - smoothed residual of the maximum velocity in the default monitor region normalized by by its maximum value.

The default values of convergence tolerance are conservative and defined such that in most cases the results should converge to the steady state solution in reasonable time. However, experienced users are encouraged to change them. Setting value of the convergence tolerance to 0 disables checking convergence for the respective criteria.

• 3.7.8.15    Timestep code (STEP)

Note:

Only available if Show advanced is checked.

The value set for Timestep code is saved in the scenario file as STEP. It is possibile to specify different time stepping options, normally to impose additional restrictions on the time step length. The values accepted by STEP are summarised in the following table.

Table 3.22: Options regarding the time stepping, specifiable with the STEP keyword in the cs-file. The options having a = require a real value of the unit specified in the table.

• 3.7.8.16    Special control keys (KEYS)

Note:

Only available if Show advanced is checked.

Any values entered as Special control keys are saved as KEYS in the scenario file. This provides the option for entering setup file options directly in CASD, e.g.

AMUL=0.6e-5

sets new value for the laminar viscosity. Multiple values are accepted using comma separation in the cs-file:

KEYS = "PR_BUO=0.9,AMUL=0.6e-5"

This string sets a new value for the Prandtl-Smith number in buoyancy term and sets a new value for the laminar viscosity (default AMUL=2.0e-5).

KEYS="PS1=01" removes the criterion in FLACS-CFD that the maximum speed cannot exceed sonic speed (imposed due to the porosity concept) and ensures that FLACS-CFD can represent supersonic flow.

This is essential for the proper description of the shock wave that results from a vessel burst with high initial pressure.

KEYS="RESET=11" ensures the consistent conversion of the three variables MIX, H, and TAU (cf. the guidance about the conversion option for rdfile utility), and also resets the turbulence level to quiescent (either the default or specifically set values of KIN0, EPS0). KEYS="RESET=10" also requires consistent conversion of the three variables, but turbulence is not reset to quiescent. Finally, KEYS="RESET=01" resets the turbulence level to quiescent, but no consistent conversion of the three variables MIX, H, and TAU is carried out.

KEYS="KIN0=1.0E-03" sets the quiescent level for turbulent kinetic energy per unit mass (here, for example, to the value 10-3 [m²/s²]).

KEYS="EPS0=1.0E-03" sets the quiescent level for the rate of dissipation of turbulent kinetic energy per unit mass (e.g. to the value 10-3[m²/s³] in the above specification).

It is possible to change the constants in the k - ε turbulence model by setting new values for:

CMY Changes Cµ in the equation for effective viscosity . Default value = 0.09.

CEPS1 Changes C1ε in the equation for production of dissipation. Default value = 1.44.

CEPS2 Changes C2ε in the transport equation for dissipation. Default value = 1.92.

CEPS3 Changes C3ε in the equation for production of dissipation. Default value = 0.8.

PR K Changes σ_k in the transport equation for turbulent kinetic energy. Default value = 1.0.

PR EPS Changes σε in the transport equation for dissipation. Default value = 1.3.

PR FMIX Changes σfmix in the transport equations for mixture fraction, fuel and enthalpy. Default value = 0.7.

PR BUO Changes σ_b in the equation for turbulent production due to buoyant forces. Default value = 0.9.

Warning:

FLACS-CFD is only validated using its default values. Do not change the constants in the turbulence model and transport equations without good reason and careful consideration.

• 3.7.8.17    MODD

This is a parameter that may be used to determine how often data for scalar-time plots are written to the results file during a simulation: data are namely stored every MODD time steps. CASD default is set to 1. This variable does not influence simulation results, only the amount of data stored.

This is normally not used in explosion simulations, but a value of MODD=10 (or higher) may be used for long dispersion simulations.

• 3.7.8.18    NPLOT

This is a parameter that may be used to determine how often data for field plots are written to file during a simulation: data are namely stored at given fuel levels where NPLOT is the number of fuel levels equally spaced between zero and a maximum. Fuel level is defined as the current total mass of fuel divided by the initial total mass of fuel. This output mechanism is not active in the case of a gas dispersion simulation (leaks are specified). This variable does not influence simulation results, only the amount of data stored.

• 3.7.8.19    DTPLOT

This is the time interval (in seconds) for field output. This is useful in gas dispersion simulations and also in gas explosion simulations when frequent output is required. The field output file will become very large if DTPLOT is set small. This variable does not influence simulation results, only the amount of data which is stored.

• 3.7.8.20    Incompressible

Note:

Only available if Show advanced is checked.

This parameter turns on the incompressible solver in Flacs.

• 3.7.8.21    Wall functions (WALLF)

Note:

Only available if Show advanced is checked.

This setting is saved in the scenario file as WALLF. This is a control switch that specifies the use of wallfunctions in FLACS-CFD. Wall-functions are used to resolve the effect of momentum and thermal boundary layers on the momentum and energy equations in near wall regions. In the scenario file the following turns Wall-functions on and off:

• •    0=OFF

• •    1 = ON

The CASD default value of WALLF is set to 1. This parameter will influence the simulation results.

When WALLF=1, wall functions are implemented, following the theory in (Sand & Bakke, 1989). A slightly modified version of this wall-functions procedure is employed when WALLF=2. However, no validation work for WALLF=2 is available.

The default value of WALLF=1 should always be used.

• 3.7.8.22    Heat switch (HEAT SWITCH)

Note:

Only available if Show advanced is checked.

This setting is saved in the scenario file as HEAT SWITCH. This parameter controls activation of the thermal attributes on objects in Flacs.

Except for fire simulations, the default choice is off as large scale explosions are not much influenced by heat loss. Turning on HEAT SWITCH will let walls and objects have background temperature, and if gas temperature changes, some heat transfer into or out of gas will take place. This is useful for small-scale confined explosions and dispersion with important heat effects. This can be combined with radiation models to account for radiative heat losses. For fire simulations the default choice is on. When deactivated, no heat radiation is calculated.

If HEAT SWITCH is activated, all solid surfaces will be initialised with the ambient temperature. Further heat objects can be specified at different temperatures using the Heat file.

For both Gas explosion and fire simulations, the radiation model can be activated in the separate Radiation scenario section. When the Radiation model is enabled, the HEAT SWITCH is activated in the solver (override the cs-file settings).

See also:

Refer to Radiation model for a more detailed description.

• 3.7.8.23    Split CGNS (SPLIT _ CGNS)

Note:

Only available if Show advanced is checked.

This setting is saved in the scenario file as SPLIT CGNS. This parameter controls splitting of the CGNS file. If splitting is disabled, then all data are written to a single < JOB> .cgns . By default, splitting is enabled for all 1D, 3D and Dump output. When splitting is enabled, the main CGNS file < JOB> .cgns contains links to many smaller, incrementally written output files in the <JOB> .output/ directory. The default setting addresses most of the issues common for large binary files: i.e., risk of data corruption, incremental downloads, and ease of archiving.

• 3.7.8.24    Convergence strategy (CONVERGENCE STRATEGY)

Note:

Only available if Show advanced is checked, and if the field alredy exists in the file.

This setting is saved in the scenario file as CONVERGENCE STRATEGY. This parameter controls activation of the rewind-restart feature

• • automatic rewind and restart of the simulation with reducted time step in case of convergence errors ('LARGE MASS RESIDUAL' condition). By default, the rewind-restart feature is enabled -CONVERGENCE STRATEGY=1.

• 3.7.9    Time dependent CFL numbers

This section in the scenario menu allows experienced users to prescribe CFL numbers that vary during the course of a simulation. The values are written to a cn-file for the current job number.

See also:

Time dependent CFL file

• 3.7.10    Dump/load settings

A runtime simulation control file (cc-file) can be written from CASD using the Dump/load settings section. To open this section of the scenario menu, right-click in the scenario menu, then select Dump/load settings.

Figure 3.21: Right-click into the scenario menu to activate the Dump/load settings section.

In the left column of the editor, you can insert cc-file keywords using a drop-down menu. In the right column, the corresponding numerical value is set. For adding or removing rows from the cc-file, right click

in the dump/load settings editor, then select Add row or Delete last row. Note that NDUMP must not be set to 8887 or 8888 since these are reserved dumpids that are used for creating restart data dumps.

IDUMP FDUMP

TOUTF

Command

NDUMP

TDUMP

NDUMP

NDUMP

TDUMP ~

NLOAD-

NDUMP

TDUMP

Command

Value

Value

"DUMP

卜                 Dumpload settings

卜                 Dumpload settings

Figure 3.22: Left: to add or delete rows right-click in the dump/load settings menu; right: the relevant command can be chosen from a drop-down menu, and the associated value entered in the right column.

Attention:

When saving the scenario, the cc-file is written only if the Dump/load settings menu is enabled. If the scenario is saved while the Dump/load settings menu is disabled, then any existing cc-file is deleted!

• 3.7.11    Boundary conditions

In the Boundary condition menu, you must specify boundary conditions for the outer boundaries of the simulation domain. The lower boundaries in X-, Y-, and Z-direction are denoted by XLO, YLO and ZLO respectively, and the upper boundaries likewise by XHI, YHI, ZHI. Recommended boundary conditions are as follows:

EULER: Euler equations

NOZZLE: Nozzle formulation

PLANE WAVE: Plane wave condition

WIND: Wind inflow or outflow

The SYMMETRY boundary condition is generally not used for realistic geometries. In addition, it is also possible to choose EQCHAR, and BERNOULLI, but these boundary conditions are generally not recommended.

Remarks:

• •    For most explosion simulations, EULER can and should be used.

• •    For wind and dispersion simulations, the NOZZLE boundary condition (similar to EULER) is more robust.

• •    The PLANE WAVE boundary condition is recommended for explosions in low confinement and for far field blast propagation. The boundary must be positioned far away from the explosion (flames should not reach the boundary and the domain should be large in comparison to the expanded cloud size).

• •    For modelling the surface of the sea or ground, it is recommended to use a solid surface together with either the EULER or the NOZZLE boundary condition.

• •    Different boundaries do not need to have the same condition.

• •    Boundary conditions try to model what happens beyond the boundary. Except for solid walls, this is not straightforward. Sometimes the boundary condition will disturb or even destroy a simulation. Then you should:

• 1.    Ensure that the chosen boundary conditions are appropriate for the problem.

• 2.    Consider increasing the Simulation volume and moving the boundaries to regions where the gradients that cross the boudaries are shallower.

Table 3.23: Recommended boundary conditions per simulation type.

The details of various boundary conditions are given below.

• 3.7.11.1    Euler

The inviscid flow equations (Euler equations) are discretised for a boundary element. This means that the momentum and continuity equations are solved on the boundary in the case of outflow. The ambient pressure is used as the pressure outside the boundary. A nozzle formulation is used in the case of inflow or sonic outflow.

Warning:

The EULER boundary condition may give too low explosion pressures in unconfined situations due to reflections from the boundary. In such cases, the Simulation volume should be extended and the Plane wave boundary condition should be applied.

• 3.7.11.2    Nozzle

A nozzle formulation is used for both sub-sonic inflow and outflow and sonic outflow. This condition is suitable for porous areas with small sharp edged holes or grids (e.g. louvres and gratings). A discharge coefficient is calculated from the area porosity and a drag coefficient. NOZZLE condition has shown to give a bit higher explosion pressures than EULER, but it is more robust.

Warning:

The NOZZLE boundary condition may give too low explosion pressures in unconfined situations. In such cases, the Simulation volume should be extended and the Plane wave boundary condition should be applied.

• 3.7.11.3    Plane wave

This boundary condition was designed to reduce the reflection of the pressure waves at open boundaries that occurs when using EULER or NOZZLE. The pressure wave reflection is caused by setting a fixed pressure at the boundary. The PLANE WAVE boundary condition extrapolates the pressure in such a way that reflections are almost eliminated for outgoing waves. However, the outflow is more restricted than for the EULER or NOZZLE conditions.

Attention:

The pressure may stabilise at a slightly elevated level after an explosion. For low confinement scenarios, it is recommended to use the PLANE WAVE boundary condition and it is important that the grid recommendations are followed to ensure that there is sufficient distance between the total simulation boundary and the combustion region (or the high pressure region for blast scenarios) to avoid any unphysical boundary effects.

Warning:

In semi-confined situations where the boundaries are close to the vents, PLANE WAVE should not be applied. PLANE WAVE boundary condition requires a large simulation volume to work and flames should never reach the boundary.

• 3.7.11.4    Wind

The WIND boundary condition models an external wind field. Velocity and turbulence profiles are specified at the wind boundaries, either by setting some turbulence parameters manually or by choosing one of the atmospheric stability classes, see Pasquill class. The WIND boundary condition is particularly applicable to dispersion scenarios. It is possible to apply WIND both on inflow boundaries and on boundaries where the flow is parallel to the boundary.

Warning:

In cases where a generated internal flow has a strong impact on the boundary flow, e.g. gas explosions, WIND should not be used.

Figure 3.23: Specification of Wind boundary condition

• 3.7.11.4.1    Wind wizard The wind wizard can be used to set up the boundary conditions if one or more of the boundary conditions are wind. The wizard can be launched from the Run Wizard->Wind wizard button available in the Scenario Settings section.

Wind setup

Set wind direction in degrees from north and wind speed

| < Back Finish Cancel

Figure 3.24: Using the wind wizard.

The wind wizard will set the boundary conditions according to the guidelines.

• 3.7.11.4.2    Wind speed WIND SPEED, U0, is the velocity on the boundary at a given Reference height. It is possible to set WIND SPEED to positive, zero or negative values, but Gexcon recommends to set a positive value and use the Wind direction parameter to specify the direction of the wind. In case of no wind, consider to use another boundary condition. A uniform velocity profile is obtained by setting the Reference height equal to zero. Then the total volumetric flux over the boundary is as follows:

V = U0 £2 An^n n

• 3.7.11.4.3    Wind direction WIND DIRECTION is a vector and each component may be given a positive, zero or negative value. The sign of this parameter determines the flow direction. A positive value means wind flow in positive direction, that is inflow over the lower boundaries and outflow at the upper boundaries. Wind at an angle different from axis directions may be specified using the WIND DIRECTION vector.

• 3.7.11.4.4    Relative turbulence intensity RELATIVE_TURBULENCE」NTENSITY, It, is the ratio

between the isotropic fluctuating velocity, u’，and the mean flow velocity U°:

It is used to calculate the value for turbulent kinetic energy, k = 3/2u’², at the boundary.

Attention:

It is not necessary to set RELATIVE TURBULENCE INTENSITY for inflow boundaries when a Pasquill class is specified. When a Pasquill class is set, FLACS-CFD will automatically create profiles for velocities and turbulence parameters at the boundary.

• 3.7.11.4.5    Turbulence length scale TURBULENCE_LENGTH_SCALE, 'lt is a typical length scale at the boundary. It is used to calculate the rate of dissipation of turbulent kinetic energy at the boundary, e:

  £

  
  

  Gk^3/2 'lt

  
  

  (3.4)

  
  

It is important that the turbulence length scale is not assigned too high a value. As a guide, it should not exceed 10% of the smallest gas cloud dimension or 50% of the grid cell size. A turbulence length scale is not required when a Pasquill class is set.

• 3.7.11.4.6    Wind buildup time WIND BUILDUP TIME is the time used to increase velocities on the boundaries from zero to WIND SPEED. A value for WIND BUILDUP TIME larger than zero gives a smooth start of the simulation. It is recommended to use WIND BUILDUP TIME for simulations with the incompressible solver, which may depend on the increased numerical stability obtained by a gradual increase of the wind speed in the initial phase. This is normally not a problem with the compressible solver. When the steady-state solver is enabled, WIND BUILDUP TIME is ignored and the velocity field is initialized with no gradual buildup.

• 3.7.11.4.7    Best practice

• •    Significant distance from the geometry to the simulation boundary is recommended (2-3 times the dimension of the facility)

• •    WIND on parallel and inflow boundaries and NOZZLE for outflow (however, use NOZZLE for +Z boundary in case of hot air releases to allow for outflow)

• •    Make sure that NOZZLE boundary is not too near, otherwise the wind will get diverted and find the easiest way out. A typical grid spacing may be 1-1.5 m, with stretching to enlarge cells away from the facility

• •    the EULER or NOZZLE boundary condition should be used for the ground/sea level, together with a solid surface.

• 3.7.11.5    Fluctuating wind

Using a setup file, you can also specify a fluctuating wind field as boundary condition. By using fluctuating wind fields it is possible to mimic time-varying wind conditions. Two different frequencies in each horizontal direction and one in the vertical direction can be used:

VERSION 1.1

$WINDGUST

USE=.TRUE.

$END

To change the frequencies of the fluctuations, more options must be specified:

VERSION 1.1

$WINDGUST

USE = .TRUE.

AMP = 2.40, 1.90, 1.84

, 2.40, 1.90, 0.00

TAU = 15.0, 10.0, 10.0

, 70.0, 50.0,  0.0

$END

Two different fluctuating periods are assumed along (15 s and 70 s) and across (10 s and 50 s) the wind direction. In the vertical direction a single period of 10 s is used. Fluctuations are done as harmonic periods with average velocity fluctuation equal to 2.4 (along), 1.9 (across) and 1.3 (vertical direction; here the constant is multiplied by 2 since only one period is used) times the friction velocity, u^∗.

Remarks:

Except for in model validation studies, fluctuating wind fields are not used very often.

• 3.7.11.6    Using TRACER mode when simulating dispersion

In 'tracer' mode Flacs will only solve a passive transport equation. This option can be useful when a dispersion of neutral gas (or small quantities of gas) shall be simulated in an established wind field. Below is an example of how to enable the tracer mode using the Setup file :

VERSION 1.1

$SETUP

KEYS="TRACE=T:100,DT_MUL=Y:5"

$END

The above setup file (or the KEYS defined in the scenario file) will simulate normally until time=100 s, thereafter only the fuel transport equation will be solved (flow field will be kept constant). When the flow field equations are switched off at 100 s, the time step is at the same time increased by a factor of 5 if using the DT _ MUL=Y:5 string.

Warning:

This option should be used with care!

• 3.7.11.7    Effect of temperature gradients

To simulate the effect of an inversion layer, it is possible to define a cold or hot temperature region (layer) in FLACS-CFD. One can for instance define a cold valley by using the setup file as described in previous sections. Boundary conditions can not take a temperature profile.

• 3.7.11.8    General considerations for boundary conditions

It is generally advantageous to place the outer boundaries of the simulation domain far away from the geometrical extent, but limitations of memory and computing speed may restrict the practical size of the problem, and in most cases one is forced to compromise between quality and cost.

• 3.7.11.8.1    Solid wall boundary The solid wall boundary condition is straightforward to model. The velocity vectors are zero at solid walls, both in the tangential and the perpendicular directions. Hence, a zero gradient perpendicular to the boundary, or a fixed value, works well for the scalar variables. Furthermore, wall-functions may improve the modelling of the flow in near-wall regions, both at the outer boundaries and in the interior space.

• 3.7.11.8.2    External influences Obstacles that are outside the vent openings of a semi-confined volume should be included in the total simulation volume because they may have an effect on the explosion. One effect may be that the total venting is reduced due to the external obstacles, especially if they are large and are placed close to the vents. Since the vent flow is changed, also the internal flow past obstacles is modified and the explosion becomes different (higher or lower pressure results). An effect which also may be important is the appearance of an external explosion which will start when the flame reaches any unburnt gas which may have escaped through the vent openings. The pressure waves from the external explosion will propagate back into the semi-confined volume and give rise to higher pressures there. The strength of the external explosion will depend on the local turbulence in the external space, this again depends on the properties of the vent openings and on any obstacles which may be positioned in the external space.

• 3.7.11.9    Boundary condition at the sea (or other liquid) surface during an explosion

When simulating an explosion above the sea, the sea surface is generally modelled as a rigid, totally blocked surface (a solid plate with area porosity equal to zero). In the real, physical world, it is likely that the water surface would yield to some extent when hit by a blast wave (despite the water itself being close to incompressible). However, the sea surface is generally expected to move only a limited distance during the time frame of a blast wave hitting it (period of pressure pulse is typically of the order of 1-2 hundred milliseconds), and this is unlikely to be sufficient to significantly affect the simulated overpressure in the central region of the explosion (assuming that there is some distance between the sea surface and the central region). Similar arguments can be made for other liquid-gas interfaces.

• 3.7.11.10    Boundary conditions for explosion after dispersion

The following approach is recommended when running an explosion simulation based on dispersion dump file.

• •    Do not stop the release before ignition

• •    Keep the boundary conditions

• •    Make sure the boundaries are sufficiently far away so that the explosion can develop properly before blast waves hit the boundary.

There may be concern about reflections of pressure from WIND boundaries, however at the time the pressure waves hit the boundaries one should be careful trusting the continued pressure curves also with EULER due to the strong negative reflected pressure sent back into the domain.

What one will experience with this suggested best practice is that everything is fine until pressure waves hit and get reflected from the WIND boundary. If the boundary conditions are changed one will see unphysical behaviour immediately when the explosion simulation starts.

• 3.7.12    Initial conditions

Initial conditions set values for turbulence fields, temperature and pressure at the beginning of the simulation. Information about the gravity conditions, parameters for the atmospheric boundary layer and the composition of the air is also set here.

The default values are as follows:

Attention:

Gexcon recommends that the default values are used for all explosion simulations where the appropriate values are not known.

• 3.7.12.1    Up-direction

This is a three-component vector defining the upward direction, i.e. opposite of the acceleration due to gravity. The three components denote the spatial components x, y, and z, respectively. It is possible to define any direction, not only directions aligned with the main axes. The vector does not need to be of unit length.

• 3.7.12.2    Gravity constant

GRAVITY CONSTANT is the magnitude of the gravitational acceleration, normally 9.8m/s². Setting a zero value for this parameter means that there are no gravitational influences on the flow. Panels with inertia are also influenced by this parameter if the direction of panel release is in the direction of the Up-direction, see also Pressure relief panels .

• 3.7.12.3    Characteristic velocity

CHARACTERISTIC VELOCITY, U0, is the mean flow velocity, and is used to find values for initial turbulence fields. It should take a positive or a zero value, see also Initial turbulence for the equivalent gas cloud.

• 3.7.12.4    Relative turbulence intensity

RELATIVE TURBULENCE _ INTENSITY, IT, is the ratio between the isotropic fluctuating velocity, u’, and the mean flow velocity, U0 :

The initial value for RELATIVE_TURBULENCE INTENSITY is used, together with Characteristic velocity, to calculate the turbulent kinetic energy, k = 3/2u’², at the beginning of the simulation, see Initial turbulence for the equivalent gas cloud.

Remarks:

If RELATIVE TURBULENCE _ INTENSITY is set to zero and a Pasquill class is provided, then the initial values for the turbulent kinetic energy, k, and its dissipation, ε, are set to be similar to their values at the wind boundaries.

• 3.7.12.5    Turbulence length scale

TURBULENCE_LENGTH_SCALE, 'lt, is a typical length scale that is used to calculate the dissipation rate of the turbulent kinetic energy, £：

C产 'lt

It is generally around half of the hydraulic diameter for internal flows. It is important that the initial value for the TURBULENCE LENGTH SCALE is not assigned too high a value. As a guide, for explosion simulations it should not exceed 10% of the smallest cloud dimension or 50% of the grid cell size, see Initial turbulence for the equivalent gas cloud.

When the initial values for all three parameters:

• •    CHARACTERISTIC VELOCITY,

• •    RELATIVE TURBULENCE INTENSITY, and

• •    TURBULENCE LENGTH SCALE,

are set to the 0 and no Pasquill class is provided, then the turbulent kinetic energy per unit mass, k, is set to 0.001 m²/s² and the dissipation rate for the turbulent kinetic energy, £, is set to 0.001 m²/s³ (these default values may be changed using a setup file).

If the inital values for all three parameters are set to positive values, then initial values for k and £ will be calculated and used in preference to the default values (if k and £ are calculated to be exactly zero, then FLACS-CFD will set them to a very small number to prevent instability).

• 3.7.12.6    Temperature

The initial temperature, T0 in °C. The default value is T0 = 20.0°C

• 3.7.12.7    Ambient pressure

AMBIENT PRESSURE, P0 is the initial pressure in the simulation and the pressure outside the simulation volume. The default ambient pressure is 玲=100000 Pa = 1 bar.

• 3.7.12.8    Air

AIR is used to define the composition of the air. "NORMAL" denotes a standard composition of 20.95% oxygen and 79.05% nitrogen in mole fractions. The composition of air can be changed by setting an other oxygen content, either as a mole fraction:

AIR         "25%MOLE"

mass fraction:

AIR         "10%MASS"

or volume fraction:

AIR         "10%VOLUME"

Changing the air composition will influence the lower flammability limit and upper flammability limit.

• 3.7.12.9    Wind boundary layer parameters

In the Wind boundary condition, the reference wind speed, Uq and the direction of the wind are specified. In addition, information about the ground conditions is needed to set inlet profiles for velocity and turbulence parameters. It is possible to specify an atmospheric boundary layer stability class, Pasquill class. Then turbulence parameter profiles are generated at the wind boundaries. If no Pasquill class is given, uniform values for k and ε are obtained on the boundary according to the expressions in Relative turbulence intensity and Turbulence length scale.

The velocity profile at the wind boundaries is given by the following expression:

u(z) = / ^ (in (T+z⁰)- %(^z)) Uq

where z is the height above the ground, Zq is the atmospheric roughness length, zd is the canopy height (displacement height) and u^∗ is a friction velocity. For the neutral and none Pasquill class, u^∗ is defined by:

___________Uqk___________

in (^(Zrf£d^{)+ Z0} ) — ^u(Zref)

ψu equals zero for none and neutral stability class (Pasquill class D), see Wind boundary.

Attention:

In FLACS v9.1 and later versions, vertical velocity and turbulence profiles start at the ground or at a given height (canopy height) above the ground. This is different from FLACS v9.0 and earlier version where the vertical profiles start at a given height (ground height).

• 3.7.12.9.1    Ground height GROUND HEIGHT is the absolute z-value where the boundary layer starts in FLACS v9.0 and earlier versions. Ground height is not used in the default model for the atmospheric boundary layer in FLACS v9.1 and later versions. The old wind boundary conditions can used by setting:

KEYS = "WIND_MODEL=2"

• 3.7.12.9.2    Pasquill class Pasquill atmospheric stability classes is a method of categorising the amount of atmospheric turbulence present. Pasquill (1961) defined six stability classes where:

A is very unstable,

B is unstable,

C is slightly unstable,

D is neutral,

E is slightly stable,

F is stable.

An overview when to apply the different Pasquill classes is given in table Pasquill stability classes.

Table 3.24: The Pasquill stability classes

Attention:

One should be careful while using Pasquill classes A-C since they are unstable, and can lead to stability problems with the simulations. The results may not be optimal when these stability classes are used and in some cases, uncontrolled turbulence “exploding” leaks is observed. Pasquill class D is recommended in these cases. They are also more sensitive to increased time step (CFL-numbers) than Pasquill classes D-F. It is recommended to choose Pasquill class D instead of A, B or C.

• 3.7.12.9.3    Ground roughness GROUND ROUGHNESS, z₀, refers to the aerodynamic roughness length. Typical values for z₀ are given in table Typical values for aerodynamic roughness length. z₀ should not be larger than the control volume height close to the surface. The aerodynamic roughness length should not be mixed with pipe roughness etc., but a rule of thumb is to relate z0 to the average height εg of the surface irregularities by zo = £g/30.